TopSolid TopSolid'Design. TopSolid Design 2006 Training Guide

Transcription

1 TopSolid'Design TopSolid Design 2006 Training Guide i

2 2006, Missler Software. 7, Rue du Bois Sauvage F Evry, FRANCE Web : info@topsolid.com All rights reserved. Information is subject to change without notice. No material may be reproduced or transmitted in any form or by any means, electronic or mechanical, for any purpose without the express written permission of Missler Software. TopSolid is a registered trademark of Missler Software. TopSolid is a product name of Missler Software. The information and the software discussed in this document are subject to change without notice and should not be considered commitments by Missler Software. The software discussed in this document is furnished under a license and may be used or copied only in accordance with the terms of this license. ii

3 Foreword...1 Pre-requisites...2 About the course and manual...2 About the software...2 Where to find files to start?...3 General...5 The TopSolid Interface...6 Functions...8 Shaft...21 Cover Plate...29 Body...37 Piston...47 Connecting rod...53 Arm...55 Yoke...65 Working with assemblies...73 Bottom-up assembly...75 Design in place 1/ Design in place 2/ Components Kinematics & Dynamics Kinematics Dynamics Surfaces Mechanically Welded Chassis Sheet Metal Work & Piping Realistic Rendering Managing the environment Managing materials Advanced rendering Managing textures and logos Importing and repairing shapes Introduction Communication difficulties Advanced Geometric Cleaning Module Non-associative mode Importing models Verify shapes Eliminate Repairs Sewing iii

4 Capping models Simplification Importing IGES Importing DWG Geometry Tool box for shapes Advanced 2D Import D Drafting Title block iv

5 Foreword 1

6 Pre-requisites Attendees should be familiar with the Microsoft Windows operating system. You should also be familiar with the principles and practises associated with mechanical design. About the course and manual This manual is intended to be used as a teaching in a classroom environment. The book itself is not therefore a self-teaching document and it does not cover every aspect in detail. The exercises in the manual are designed to be explained and supported by an experienced instructor. About the software TopSolid is a contemporary CAD product that runs in the Windows environment. TopSolid is the core product of a family of integrated software solutions developed by Missler Software that offer a global and integrated general mechanical solution for both design and manufacturing. The family of solutions includes: TopSolid Design: 3D design and surface modelling TopSolid Draft: drawing features and 2D design TopSolid'Castor: FEA analysis of structures in terms of volume beams and hulls TopSolid'Motion: dynamic calculation of motion TopSolid'Mold: mold and tooling design TopSolid'Progress: progression and stamping tool design TopSolid'Fold: design and unfolding of sheet metal applications TopSolid'Cam: 2 to 5 axis 2D/3D milling, turning and wire EDM TopSolid'PunchCut: punching, nibbling and cutting for sheet metal applications 2

7 These products share the same user interface and associative database. For each module, Missler Software offers a product with real associative CAD/CAM, thus avoiding duplication of information transfer between the engineering and manufacturing departments. The result is an impressive gain in productivity. To make all this possible, TopSolid implements a method of design using functions and components that already contain the information needed for assembling and manufacturing. About the course and manual During the course we will be modelling several parts. Ensure to save them as we will use them again in the assembly module. Where to find files to start? Some of the training lessons need files to start: they are all available from TopSolid 2006 DVD in Documentation folder followed by the product and the chapter name (e.g. Documentation\TopSolidDesign\Shaft). 3

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9 General 5

10 The TopSolid Interface Title Bar Drop down menus Function Bar System Bar Prompt Line Context Bar Graphic area Alpha Bar Status bar Provides feedback and allows the user to quickly set layers, colors etc. and set display tolerances and invisible parts. Click directly onto the value to change it.. Snap grid on or off Manage layers and transparency Edit material Cursor position Set picking mode: 3D=Spatial Pr=Projected Pl=Planar Edit display tolerance Note This will directly affect file size Hides or displays invisible items 6

11 Mouse Functions Different functions are associated with the three buttons of the mouse. Left Mouse Button (LM) : Selection of any function from the menus Selection of an element (dynamic selection) or creation of a point Middle Mouse Button (MM) : Creation of points on the current plane when clicked (advanced) Dynamic Zoom using Scroll Dynamic Pan when held down LM MM RM Right Mouse Button (RM) : The first option of the current command is accepted when the right mouse button is clicked Or the context menu of the current command is displayed when held down. Three further important uses 1. Intersection of 2 Items: To obtain the intersection of two items left click and hold LM in the graphics area away from the intersection then move the mouse over the intersection then release the mouse key; - The size of the square can be changed using the + and buttons on the keyboard. 2. Rotative picking of items: When the mouse is moved over an item, the nearest item is automatically highlighted if this is not the required item, press and hold down the left mouse button and use the right mouse RM click to allow Rotative picking through the items at the current position. When the correct item is highlighted release the left mouse LM. 3. The middle button has one more distinct property in that when drawing lines for instance it will always create a NEW point even if you click onto an existing one. 1 Here we draw 2 separate lines that join at a point. All done with the left button. If we move the common point, then we see that both lines alter to remain joined. 2 - Here we draw 2 separate lines that join at a point however the second line was drawn with the right button. If we move the common point we see that the two lines are in fact separate and can move independently. 7

12 Functions The icons There are two types of icons in Topsolid, simple icons and icons with options. The simple icons execute the function with a single left mouse click LM. The icons with options using the left mouse LM on the Icon selects the command as above. If you use a left click LM the option selected becomes the default option for the next time you use this function If you use a right click RM the default option does not change Using the Context icon bar Many of the functions are grouped together in context using the context bar (the vertical icons bar located on the left of the screen) Selecting an icon will change the functions displayed in the work bar (horizontal icons bar located under the system icon bar), and in some cases the menus are also changed when you change the current context. The buttons Input boxes for values, when TopSolid needs input from the user, it will display an empty box. In this case, the input is done directly via the keyboard. The buttons without drop down menus. These allow switching between several options. For example to draw a circle by default the option Diameter is selected. A click on the button switches the command to Radius. 8

13 Some allow the selection of options from a drop down menu. For example Transformation has a drop down box showing the other available options as shown here: Keyboard actions Left mouse down with Control enters dynamic rotation, Shift enters dynamic pan and both keys together enters dynamic zoom. The function keys in TopSolid have the following uses, as well as the normal windows functions. Key F1 F2 F3 F4 F5 F6 F7 F8 F9 F10 F11 F12 Function Online Help Information on points and elements Dynamic Zoom Dynamic Pan Dynamic rotation around X Dynamic rotation around Y Dynamic rotation around Z Cancel Dynamic rotation Dynamic Rotation Floating windows On/Off User defined shortcuts can be created using the Tools, Options menu. Typing in Coordinates Cartesian coordinates: defines coordinates whose values are absolute from the current coordinate system origin (X, Y, Z). Commas separate the values, the Z value is optional. Ex: 12,45,21 Polar coordinates: defines polar coordinates length in XY plan, angle and a height in Z (length; angle, z). The Z height is optional. Ex: 20;45,5 Spherical coordinates: defines spherical coordinates length in XY plan, angle in XY then angle in YZ view of the current direction (Length;angle1;angle2). Ex: 5;45;30 Relative coordinates: defines coordinates relative to the previous point specified the coordinates are preceded by the symbol &. Ex: &10,10,10 9

14 The compass A compass that allows changing the view orientation is available in each view. In its default position, it represents the current coordinate system orientation. Each part of the compass allows you to make dynamic actions view along a direction, centred rotation, rotation around axes, translations. In its default position, the compass shows the orientation of the current coordinate system. It is used to manipulate the view. It has sensitive parts, each of which enable dynamic actions to be performed: i.e. orientation along a direction, centered rotations, rotations along axes, translations. Transformation Area(s) to click Displacement of the view (Panoramic) Spherical rotation Rotation along an axis Rotation around X Rotation around Y Rotation around Z Modification of a view orientation View along X (Right) View along Y (Back) View along Z (Top) 10

15 The compass may be positioned anywhere in the view or hooked to an element of the document by sliding-moving its centre point. Area to click Hooking the compass to an element allows the user: to manipulate the view according to the new orientation of the compass: rotations along the hook axes to create a coordinate system on the hook (accessed via the contextsensitive menu, right button) to create a current coordinate system on the hook (accessed via the context-sensitive menu, right button) A symbolic coordinate system representing the current coordinate system is maintained at the compass default position if the compass is moved (whether hooked or left free in the view). When the compass has been moved, it may be moved back to its place at the bottom left of the screen, and vice versa, by double-clicking. The compass may be temporarily hidden via its context-sensitive menu. Use the context-sensitive menu of the default coordinate system to make it reappear. When the compass does not appear in the view (i.e. if it has been hooked to an element that has passed outside the view), it may be retrieved by clicking on the default coordinate system. Main functions presentation New document There are a selection of Templates provided for creating new documents in TopSolid Design and TopSolid Draft. User defined templates can be stored in the Config/Template directory of the software. For training we will use Associative 3 Csystems mm. Open an existing document TopSolid shows a list of files in the current folder with the extension.top and.dft and also files supported by the direct interfaces STEP, IGES, DXF, DWG, Parasolid, ACIS etc. Some direct interfaces are separately purchasable. Note: New creates a new document. The Configure button is active depending on the type of direct interface file used. Save or Save as to save as a different name 3D design files are saved with the extension.top and 2D files are saved with the extension.dft. In the title bar, if the name of the file is followed by a *, this means that there are changes to the file that have not been saved. If there is an exclamation mark it means there are some invalid elements. Files can also be saved in other formats such as STEP, IGES, DWG, DXF, etc. 11

16 Print Prints the current document. Depending of the application used you have will have different printing options. Cancel Cancels all the actions carried out within the current function but does not exit it, to quit the function press the Escape key. Undo Undo the previous action within the current command. Delete element Deletes the selected elements. The option ALL THE ELEMENTS allows, after confirmation, to clear the current document. Extract element Extract a portion or feature of an element.(e.g.: point of a contour, drill or fillet on a shape, union, boss, title block element,...). If there is an ambiguity, TopSolid will ask you to choose between them. The element or the operation is destroyed but the elements that were used to create it are preserved. Example: the extraction of a boss eliminates the boss but not the profile from which it was generated (The profile remains invisible). Insert element Insert an element (e.g. point, line, circle). Modify element Modify an element or operation e.g. contour, radius boss, transformation Move parents Move an element and its construction elements if the element is not fully constrained Topsolid will show dynamically the possible positions. Contour Creates contours over existing sketch lines, or on the grid of the active coordinate system, closed contours are automatically created when the start point is re-selected. Sketch lines Sketch lines are created relative to points or elements, the option boxes allow the change of angles etc. 12

17 Extrude shape Creates an extruded surface or solid from a profile. Generally if the profile is open a surface is created, if it is closed a solid is created. Revolved shape Creates a revolved surface or solid from a profile around the selected axis. Drawing contours There are two ways of drawing contours either by clicking point to point or alternatively by tracing over construction geometry. Simple contours To define the contour using points, lines are sketched defining the relevant points of the part. The actual dimensions / angles of the shape are defined later by dimensioning. Once the shape has been drawn you can use Modify to change the conditions at a vertex (chamfer, fillet or nothing) or between two points you can change the link type (line, arc, tangential) Depending on whether you select near an end or in the middle of a side. 13

18 Creation from construction lines: To define the contour the user uses basic sketch elements (lines, circles etc.). The dimensions of the contour depend on dimensions and positions of the sketch lines. What does parametric mean? Parametric modelling allows the part to automatically link to the basic geometry from which it was created, so that changes can be automatically updated throughout the design process. A simple example is as follows. In a traditional cad system when the operator creates a point at the intersection of two lines the point is created but if one of the lines moves later, the point does not automatically move with it. In a parametric system when the operator creates a point at the intersection of two lines it remembers this operation so that if one of the lines moves later the point is automatically updated to be at the new intersection point. Basic system Parametric system Point remains in position Point follows new condition 14

19 The coordinate systems A coordinate system allows the creation of a work plane for the construction of elements. When we start a new document (associative 3 Systems mm) there are three coordinate systems: the absolute XY one, and a XZ plus a YZ coordinate system. To change or create a coordinate system, select in the Current system system bar the function Current coordinate system then pick a face or a coordinate system. In the example, it is necessary to select the yellow face. Absolute system Numerous forms of coordinate system are available and these can be accessed from the coordinate system tool bar. NOTE This icon will allow you to set any coordinate system as the current or active one. This icon displays the coordinate system tool bar and allows the user to create a new coordinate system. If used alone the coordinate system created will NOT automatically become current, however if you use first of all, then the resultant coordinate system WILL automatically become current. The current (or active) coordinate system is drawn in a thicker outline. The most widely used coordinate systems are: Coordinate system on point Coordinate system through 3 points Coordinate system on profile Coordinate system on a profile and point. Coordinate system on face and a point Coordinate system constrained on a face Duplicated coordinate system Examples of their use: 15

20 Coordinate system on a point: Constructs a coordinate system positioned on a point, taking the orientation of the current coordinate system. Coordinate system on curve and point: Lets you to create a coordinate system that is based on a curve and a point. The curve defines the orientation of the coordinate system (XY normal in relation to the curve), the point defines its position. Constrained coordinate system on a face: Creates a coordinate system placed on a face and positioned in respect of the edges or contiguous faces. The DYNAMIC button enables searching for these edges or sides used. Note: Very convenient as the two dimensions easily allow the coordinate system to be moved later. Duplicated coordinate system: Creates a copy of a coordinate system by applying a transformation, translate, rotate etc. Systems duplicated by rotation Original system System duplicated par translation 16

21 Points Points are elements that comprise a distinct position. They are maintained during associative mode design. Points are used to join dimensions, to impose dimensional and positional constraints. In contrast, in free design mode and non associative curves mode points are deleted immediately as soon as the function is changed, as they cannot be used to constrain an element. Creation of points in TopSolid is performed in several ways: First of all, during construction of b-spline curves, the user is actually tracing points without realizing it. These points include, for example, the centre of a circle that is placed on the grid, a line that is joined to the end of an existing curve, etc. The other method is to use a specific point creation function, by choosing the menu Tools, Points or the points tool bar. The most widely used points systems are: Intersection point: point at the intersection of 2 curves. Middle point: a point created between 2 other points. Centre point: a point in the middle of an element. (lines or circles). Point on a curve: create a point attached to a curve. Barycentre point: a point at the centre of gravity. Using points Duplicate point: a duplicated point which is translated from the original. Axis-curve/plane-face intersection point: The Intersection point between an axis/ curve axe and a plane/face allows you to create an intersection point between a curve or an axis an a face or a plane. Intersection point: creates an intersection point between curves. Middle point and Centre point: creates a centre point of the arcs and then the middle point between the two centre points. 17

22 Point on a curve: creates a point on the upper edge of the cylinder. It is possible to combine the coordinate systems with points on coordinate systems with icons showing a red point. For example, in the following case, a coordinate system on face and point will be created, and the point will correspond to a middle point between 2 other points (which are actually the centre points of the 2 circles). Middle point Face Transformation and associativity A part or element can be transformed or moved from one place to another. Or it can be duplicated either single or multiple) The most common propagations are translation and rotation, but it may be symmetry, double symmetry, homothetic, rectangular, etc. The important question with respect to the associativity mechanism is: what happens to the parents when such a propagation is applied? There are numerous options for the user to choose from and the correct choice will depend on the required outcome. Move and turn functions These 2 functions apply the translation and rotation to the parents of the selected element. The entire element will be affected. For elements such as lines or circles and simplistic shapes this has very little impact. But if a part that you are applying a move and turn function to has several other parts based from it the result will also be applied to those parts this may not give you the desired effect. Repeat or duplicate? When applying a propagation, it may be useful if the number of resulting elements were to be a parameter, so that it can be changed later. The Edit, Repeat function allows for this, however the Edit, Duplicate function does not (but it is less complex in terms of associativity). The main effect of the Repeat function is to create a top level element other the copies, and the copies themselves are in fact considered as completely new elements. For example, you may have to detect an element inside the repetition to access it. Repeat (or not) any further modification to the original? The duplicated or repeated elements may be allowed to follow any new operations (chamfer, holes,...) applied to the original. This has to be set by the user. By default, the subsequent operations to the original will applied on the duplicated or repeated elements too. Linked or independent copies? 18

23 If you simply want to copy an element without any link back to the original, use the Copy without reference option.this has the effect of breaking the associativity between the original and its copies. 19

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25 Shaft Topics covered: Create a simple contour. Dimension/Half part dimension. Revolved solid. Extruded solid. Trimming with curves. Creating a reference system. Subtraction (cutting). Chamfer & Fillet. Simple part drawing. 1 Starting a new design document Open a new file then select a new design document and select a template. Click on the profile icon in the context bar. The Profile command will start automatically. NOTE: this will only happen the first time you select the context menu. Use the profile tool to draw the profiles shown below. Create the profile by clicking free points but use the cursor feedback information as a guide. Start your profile on the coordinate centre point. To close a profile either click onto the first segment or click onto the last (previous segment). Then end the open profile (shown in grey line). Click STOP. 2 Dimensions Dimension both contours as shown, use the and for diameters. 3 Create the revolved solid Activate the shapes context menu select the revolved shape icon. 21

26 Select your curve then select the horizontal base as your rotation axis. Click OK to accept a 360 degrees rotation. NOTE: Changing the direction (in this case) will have no effect. 4 Adding the chamfer Click on the chamfer icon. Choose the chamfer type as LENGTH/LENGTH, enter 1mm in the first length box then click onto the front edge of the shaft. 5 Limiting with a profile (trimming) Click on the trimming icon. For the shape to trim select the shaft. For the trimming shape select the open profile. 22

27 Ensure that the large red arrow is pointing towards the inside of the curve (area to delete) then click OK. Cut the keyway. Select the menu Tools, Coordinate system. Select XZ. Click SET AS CURRENT then top view. Draw and extrude the key. Draw a circle using the circle icon. Radius 8mm, Centre point 17,8,0. Extrude the circle to 4mm. Activate the shape context menu then select the extrude icon. Click on the circle. Click on the NORMAL button to change it to CENTRED, then type in 4mm. 23

28 6 Subtraction Click on the subtraction icon. Select your shaft as the shape to modify. Select your extruded circle as the tool shape to use. NOTE: Use the Esc key to exit the command afterwards. Save your file and name it Shaft. 7 Create a drawing of the shaft Open a new draft document. Use the New document icon then select Draft as the document type and select a Associative A4 vertical mm template. Your windows will tile vertically automatically. NOTE: This only works if there is only one design document open. In which case use the tile windows icon. 24

29 Select the main view icon. Click on the shaft. Orientate the view with the green arrows and type a new scaling factor if required, select OK to accept. Position the view onto the sheet and left click. Select AUXILIARY VIEW (or right click) to create the projected and isometric views. Save your file and exit. NOTE: By default the name of the file will be Shaft.dft. You may of course choose another name. 25

30 Modifications to the shaft 8 Drilling holes Use the menu file Open icon and select the file Shaft.top. Click OK. We will add 2xM4 tapped holes onto the face of the cut-out: Select the drilling icon, select the face and use the cursor to position the first hole position. Notice the green and yellow dimensions. Select hole+tapping. 26

31 Select M4, tick Through and OK. The design calls for 2 holes. So use the PROPAGATE button to pattern the second hole. Select LINEAR. Select one of the long edges to define the propagation direction. Ensure the direction arrow is correct. The total distance is 25mm. Total number is 2. Save your file. Open the shaft drawing file Shaft.dft. 27

32 9 Local Section Let s add a local section to the main view. Activate the views context menu and select the local section icon then select the main view. Select B-SPLINE. Draw the spline by clicking points, then STOP. NOTE: You could in fact draw any shape first, then select CONTOUR. Click onto the outline of the shaft. Result. 10 Drilling dimensions Activate the dimensions context menu then select the hole dimensions icon. Select any element belonging to a machined hole, then place the dimension. Save the file. 28

33 Cover Plate Topics covered: Cylindrical primitive. Drilling. Coordinate systems. Points. Propagation. Chamfer. Feature tree. Detail drawing. 1 New document Open a New document select Design as the type. 2 Cylinder Activate the shapes context menu then select the cylinder icon. Enter 50mm. Select Z+. Enter 6mm. Enter 0,0,0. 29

34 3 Drilling Drill a Ø14 plain hole in the centre of the cylinder. Select the drilling icon then select the face, fill out the drilling dialogue for a plain 14mm hole. 4 Sketch for the PCD Change your line color and style. Draw a circle diameter 38mm centred on the 0,0 point. Draw a vertical sketch line using through 0,0. Select CHANGE TO VERTICAL then ENTER or click the centre point. 5 Points Click on to activate the points menu bar. Select the curve intersection icon. Click on the circle followed by the vertical line. Pick close to actual intersection point to identify which one of the two possible solutions you require. 6 Place the coordinate system Click on the icon to activate the coordinate systems menu bar. 30

35 Select the coordinate system on a point icon click on the point created at the intersection.. Then Drill Ø5 holes on the newly created coordinate system. Select COORDINATE SYSTEM. Click onto the coordinate system then onto the face of the cover plate. Select PROPAGATE. Select CIRCULAR. Select Z+ (or select the vertical side of the cover plate). 31

36 Right click to accept 360. Type 3 and Enter. Esc to exit the command 7 Chamfer, place a 1mm x 45 cham- Select the chamfer icon fer around the top edge. 8 Feature tree To open the feature tree click on the left hand side of the graphics window, then onto your shape. Alternatively left click and drag on the left hand side of the graphics window to open it, then right click in this area and select Edit then click on the shape. Change the chamfer 1.5mm. Change the number of holes to 6. Change the diameter of the centre hole to 10. Now change them all back to their original values with Save the file as CoverPlate.top. 32

37 9 Detail drawing of the cover plate Open a New document with select Draft as the document type. Create a Main view. 10 Axis Drawing axis may be placed one at a time or in this case we will do all the axis on the part automatically. Select PROJECTED AXIS. Select your view. Select AUTOMATIC. Then OK. 11 Cross-section Select the full section icon. Select CUTTING CURVE DEFINED IN DRAFT. 33

38 Click the vertical axis. Select OK. Select OK and place the view. 12 Change the position of the A-A Click the modify tool then click the text A-A. Select FREE POSITION to put the text wherever you want it. NOTE: INVERT will change the direction of the cutting arrows. EXTREMITIES controls the position of the 2 ends of the cutting line. 34

39 13 Dimensions Dimension the holes. Dimension the chamfer with this icon. NOTE: For chamfers that are not at 45 you must use the START AND TERMINATE SEGMENTS function. Select the lines on either side of the chamfer to establish the angle and size. Put the other dimensions onto the drawing with and select the relevant lines and arcs. Save the file as CoverPlate.dft 35

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41 Body Topics covered: Cylindrical primitive Sketch contours Extrude + Unite Propagation Drilling 1 Open a new document select Design as the type 2 Cylinder Activate the shapes context menu then select the cylinder icon. Enter 75mm. Select Z+. Enter 90mm. Enter 0,0,0. 37

42 3 Add the feet Draw a construction circle of Ø100. Draw a vertical construction line through 0,0. Draw a circle of radius 12.5 on the top intersection point of the circle and the line. Use the cursor slide selection technique to find the intersection. Draw 2 vertical lines tangent to both sides of the circle. Draw a horizontal line at 0,30. Change your line color and style and draw a contour tracing over the construction lines. by 38

43 Extrude the contour 8mm vertically upwards. NOTE: Click on the red arrow to change the extrusion direction. Join the two parts together with the Unite icon. 4 Propagation Propagate the feet around the base with. Use a CIR- CULAR PROPAGATION and the cylinder as the propagation axis. Make a total of 3 feet around 360. Drill the Ø12 holes in the feet plain drilled hole through. in the dialogue select a 5 Propagate the holes Select the PROPAGATE button then simply select the face of one of the feet. The propagation will be copied from the feet to the holes. 39

44 Drill another hole in the centre of Ø50 with a chamfer (or countersink) of Ø70 x 45. Select the top face of the body then select hole + countersinking as the hole type. Note the 2 dialogues 40

45 6 Change the workplane Select the menu Tools, Coordinate system. Select XZ. Choose SET AS CURRENT then TOP VIEW. Draw a circle of diameter 50 at 0,28. Extrude the circle by 40.5 in Z+. With the unite icon join them together. Open the feature tree and move the drilling operation so that it comes after the unite. This will have the effect of removing the obstruction from inside the hole. Close the feature tree by clicking on the edge 41

46 7 Drill the counter bored hole Ø14-25 Select the face of the Ø50 cylinder. Choose hole+facing and fill out the dialogues as shown.. 8 Drill and tap 3 holes M4 Set the current coordinate system onto the face of the 50mm cylinder. Select the normal (or top) view. Draw a 38mm diameter circle at 0,0. Place the axis lines on the circle. 42

47 Create another coordinate system at the intersection between the circle and the horizontal axis with (use the cursor slide again if you wish). Select the drilling icon. Select COORDINATE SYSTEM then click on the new coordinate system, then the cylinder face. Choose the tapped hole and fill out the dialogue as below (note the depth of the holes). Propagate the holes with a circular propagation using the 50mm cylinder as the propagation axis. We need 3 holes. Finally put 1mm fillets around the edges and corners of the feet as shown. Save the file as Body.top. 43

48 9 Detail drawing of the body Open a new document with select Draft as the document type. Create a main view and projected view as shown. 10 Section view Click on the section icon then onto the main view. Click the circle; the circles axis will appear automatically, use the vertical line of the axis as the cutting contour. Select OK. Set the hidden lines to HIDDEN then OK. Place the view on the drawing. 44

49 11 Partial section Draw the projected axis. Draw a line from the centre of the 50mm hole to the centre of the drilled hole in the foot. You can use the trim function just outside the foot (as shown). to extend as well as shorten. Select the line and click on a point Select MAKE TRIM. Click on the partial section icon. Select the view. Click on the line we have just drawn. Select OK. Set hidden lines as HIDDEN, then OK. You will see that the view is incorrectly aligned, go back and select NO and YES as shown. Position the view correctly and Esc to exit the command. 45

50 Dimension the rest of the drawing as shown. 12 Tolerance reference Activate the dimensions and detailing context menu then. Click on the line to use as a reference and place the symbol. 13 Geometric tolerance Select the geometric tolerance icon. Select the correct type of symbol from the list then OK. Click on the element you wish to refer to. Click onto the reference letter A, then STOP. Save the file as Body.dft. 46

51 Piston Topics covered: Freehand contour. Revolved solid. Grooves. Slots. Drilling on cylinders. 1 Shape creation Open a new document select Design as the type. Draw the initial profile as shown. Dimension with. Revolve the shape with. 2 Groove Select the groove icon. Click on the face as shown. 47

52 Click on the front face. Select OK. Enter the values d=5, D=45 and l=2 Then OK. 3 The Slot Place a coordinate system on the back face. From the coordinate system menu bar, select Constrained coordinate system on face. 48

53 Draw the axis on the circular outline. Select the slot icon. Select the face. Click on the vertical axis line. Choose the U type slot. Then OK. Type 4mm. OK. Type 10mm. OK. Select OK.. 4 Drill the Ø4 hole As the face to drill through is not planar we will need to use a coordinate system. Select the current coordinate system icon. Select ABSOLUTE COORDINATE SYSTEM. 49

54 Select the top view icon. From the points menu bar, draw a point. Place the point 5mm in from the end of the 15mm diameter. Create a coordinate system on a face and point the preceding point. face = face of the Ø15 cylinder and the point is Drill the hole using this coordinate system. Make it a plain drilled hole Ø4 through all. 5 Detail drawing of the piston Open a new document with. Select Draft as the document type. Create a main view and projected view as shown. Create a local section as shown. Draw the axis. Dimension the part as shown. 50

55 6 Adding tolerances Click on the dimension to adjust with, then select the tolerance style. Enter the values for the upper and lower limits as shown below. Before After 7 Adding Notes Activate the detailing context menu with. Then select the notes icon. Enter your text, notes and set the style, etc. Place your note on the drawing. Click on a line segment to place the head of your leader. Select STOP. 51

56 8 Shaded view Modify the view with shaded view checkbox. then tick the 52

57 Connecting rod Topics covered: Thicken. Symmetry constraints. Extruding. Propagated drilling. 1 Constrained line Draw a line with. Dimension the line. Adjust the length to 3mm. Add a symmetrical constraint about the Y axis. 2 Thicken the profile Select the thicken icon. Enter the thickness 5mm and select CIRCLES OUTSIDE then click on the line. Select OK (or right click). Extrude the contour 4mm. Drill a hole in one end Ø4mm. 53

58 Propagate the drilled hole using SIMPLE MIRROR through the YZ plane. Save the file as ConnectingRod.top. 54

59 Arm Topics covered: Sketch Contours. Modifying elements. Extrude solids. Unite. Merge (contours). Pocket. Drilling. Standard profiles. Fillets. Some advanced drawing methods. 1 Arm profile Open a new document select Design as the document type. Draw 2 circles with the circle icon and dimension change to a dotted line first. NOTE: You can draw the circles roughly then correct their size and position using the dimension tool, however it s a good idea to place the first one on the coordinate 0,0. Draw a 2 lines tangent to the 2 circles use the Contour command but use a different colour. Click the first circle. Ensure PASS ON SEGMENT is selected, click the second circle at 2 o clock and again at 5 o clock. Click on the first circle to close the profile. 55

60 2 Modify an element Click on the modify tool then select the top straight-line segment of your profile. Simply type 125mm as the circle size (no need to select the circle button) and Enter. If the arc goes the wrong way, click on the tool again and select INVERT. Repeat the procedure for the bottom arc using 70mm radius. 3 Extrude the shape Use the extrude icon extrude the 2 circles to a thickness of 11mm (CENTRED). NOTE: Use the lasso to select them both at the same time. Then extrude the contour by 5mm (CENTRED).. Unite. 56

61 Select the centre shape. Select the two cylinders. Esc to exit. 4 Merge contours Draw a circle Ø14 and a rectangle 3X5 as shown : use the RECTANGULAR option and select the two diagonal points. Hold down the right mouse key and select AUTO DIMENSION, then use SYMMETRY constraints to add a constraint on the X axis. Add a 10mm dimension to position the rectangle. Use the merge icon to merge the 2 contours together. Remember to pick the contours on the section you wish to keep. 5 Pocket With the pocket command use the profile to cut the pocket on the boss. 57

62 Select the face. Select the profile. Select Through all and OK. 6 Drilling With the drilling icon click on the face of the other boss. As the boss is circular the system will automatically select the centre. Select a plain hole then OK. 58

63 Type in 10mm for the diameter and click Through all then OK. 7 Do the drawing Use the New document icon then select Draft as the document type and select a Associative A4 horizontal mm template. Your windows will tile vertically automatically. Select the main view icon. Select AUXILIARY VIEW (or right click) to create the projected and isometric views as shown. 8 Create a detail view Click on the detail view icon. Click on the main view (shown above with a highlighted border). 59

64 Select CIRCLE. Click on a point close to the keyway then click again to open up the circle. Place the view where you want it. 9 Projected dimensions Activate the dimensions context menu then select the projected dimensions icon. Select the main view. Click on AUTOMATIC. Repeat for the other views. NOTE: These are driving dimensions, which means that they can be changed in the drawing and will directly change the model. Save the file, name the files Arm.top and Arm.dft. 60

65 10 Modify the Arm Open the fie Arm.top. To see the elements that are driving the model click on the driving elements icon. Click on the centre face. Use the circle tool to draw an arc of radius 90mm passing through the centre of the 2 circles. NOTE: change the color and line style using and. 11 Standard Profile Draw a radiused slot using a standard profile. Double click on each of the values. Type in 90mm for the radius, 10mm for the thickness and 20 degrees for the angle. Ensure the key point is set to middle. 61

66 Place the slot onto the centre of the 90mm arc. Now use the pocket command once again to cut the pocket through the arm. This time use the fillet option to add a 1mm fillet top and bottom. 12 Fillets Activate the shapes context menu then select the fillet icon. Select the four edges between the boss s and the centre section and click compute fillets. 62

67 Save the file with. Open the arm s draft document to see that it has automatically been updated with the changes. 63

68 64

69 Yoke Topics covered: Rectangular contour. Extrude. Chamfer. Drilling a face. Use your newly acquired skills to model this part yourself (it needs to fit into the cut-out on the end of the shaft and the connecting rod fits inside the slot). 65

70 A-A 2 x M4 66

71 67

72 A-A 3 holes Ø5 68

73 A-A 3 tapping holes M4x5 Counterbore Ø25x5 B-B 69

74 70

75 2xØ4 71

76 72

77 Working with assemblies 73

78 Topics covered: Assembly methods. Defining a part. Defining an assembly. Assembly using constraints. Assembly using coordinate systems. Dynamic simulation and the constraints system. Using standard components. Producing assembly drawings. Exploded views. Bill of materials and indexes. Designing in place or top down method. When bringing parts together in an assembly we can work in two different ways: Bottom up. The separate pieces of the assembly are modeled individually and then brought together to make the assembly. They are fitted together using constraints or coordinates. In place (or top down) All the parts are built in place in the same file. Design Creation of independent parts Assembly Sub-assemblies Creation of parts in place The Full assembly Creation in place of a part in its assembly context 74

79 Bottom-up assembly 1 Creating parts & different sub-assemblies We will start by making a sub-assembly of the shaft and yoke. Shaft Yoke 2 Defining a part Each component of an assembly needs to be identified and some characteristics specified. This will be of use later when we do drawings and bill of materials. Open the Shaft.top file. Activate the assembly context menu then select Define a part. Select the shaft then fill out the dialogue box as follows. Name = Shaft, reference=sh-01, Material=Steel Click OK. NOTE: If you need to modify any of the inputs later, you can select Characteristics from the feature tree. 75

80 The BOM index tab is available if you want to manually insert a specific BOM index. Save the file. Repeat the same process for the Yoke: Name = Yoke, reference=yk-01, Material=Steel Save the file. NOTE: You will by now have realized that this process (of defining the part) is prompted for each time you save a file in TopSolid. If the part you have been working on when this happens is in fact to be included in an assembly later on then of course it will be much more convenient to accept the prompt and fill out the dialogue at that point. 3 Assembly using constraints Open a new design document. Activate the assembly context menu then select Include sub assembly/part. Select EXPLORE and open the file Shaft.top. Place the part anywhere. Select STOP. Select NO PROPAGATION. Select OTHER COMPONENT. Select EXPLORE and open the file Yoke.top. 76

81 Place the part close to its final position. Select the base face of the yoke (i.e. the contact face between the two parts). Select the destination face (the flat face on the shaft). Select OK. NOTE: TopSolid has proposed a logical constraint for the two faces you selected, however the MATE button allows you to select your own constraints and positioning. Click on the cylindrical hole in the yoke. 77

82 Select the corresponding cylindrical face in the shaft. NOTE: TopSolid selects the only possible constraint (axis on axis). Click on the 2 nd cylindrical hole in the yoke. Again select the corresponding cylindrical face in the shaft. Select STOP. Open the feature tree Edit the assembly. Expand the Constraint Positioning. NOTE: During assembly In AUTO mode, TopSolid will propose the correct constraint in around 80% of cases. 78

83 Here we can add the details (characteristics) of our subassembly by selecting Assembly and right-click and selecting Characteristics.Alternatively, select Define Assembly then select CHARACTERISTICS. Save your file. Close the Shaft and Yoke files. 79

84 4 Adding a standard component Activate the assembly context menu Include standard. From the ISO library select an M4x10 cap screw, then click OK. Select the face close to the circular edge. This will orientate the screw correctly and at the same time place it in the hole. Select STOP. Select STOP. Select STOP. Again select the face close to the circular edge at the other end of the yoke. This will orientate the screw correctly and at the same time place it in the hole. Select STOP. Select STOP. 80

85 Select STOP Then Esc. The two screws will automatically be added to the assembly. Save the file. 5 Complete Assembly of the Valve Open the file Body.top. Define the part : Designation = BODY Reference = BD-01 Material = Grey cast iron Open the file ConnectingRod.top. Define the part. Designation = CONNECTING ROD Reference = RD-01 Material = Steel Open the file Piston.top. Define the part. Designation = PISTON Reference = PS-01 Material = Steel Open a New design document.. Activate the assembly context menu then select Include sub assembly/part. Find and open the file Body.top. Select OTHER POSITIONING. TopSolid will open the Body.top file automatically in order for you to select a new reference face or coordinate system. Select the Coordinate system at the top of the body (the absolute coordinate system). 81

86 TopSolid will then return to the new file. Click onto the absolute coordinate system then select NO PROPAGATION. NOTE: The body is now constrained by the position of its coordinate system. Add the Sub-assembly we did earlier (shaft and yoke). Constrain the axis of the shaft to the axis of the hole in the body. Constrain the shaft in the longitudinal direction by fixing the face on the back of the flange to the face in the bottom of the counterbore. 82

87 Define the characteristics of the assembly: Designation = Valve Reference = VN-01 Save the file. 6 Assemble the Cover Plate Activate the assembly context menu then select Include sub assembly/part. Select EXPLORE and open the file CoverPlate.top. Place it down. Select the face on the back of the cover plate then the top of the boss. Select OK. Choose the cylindrical face in one of the holes of the cover plate then a corresponding hole in the boss. 83

88 Repeat the operation for a second hole. Place 3 M4x10 cap screws in the holes. This time place one screw then propagate the rest through 360. Save the file. 7 Add the Arm Activate the assembly context menu then select Include sub assembly/part. Select EXPLORE and open the file Arm.top. Position it as follows: 84

89 TopSolid 2006 Type of constraint Axis on Axis Origin Geometry Destination Geometry Alignment on faces Alignment on the key Save the file. 8 Add the connecting rod To see the yoke more clearly we can move the body to layer 1. Do this easily by right-clicking 1 on the quick layers toolbar. Left click on the body then OK. NOTE: The part disappears because level 1 is not set as a visible layer. Activate the assembly context menu then select Include sub assembly/part. Select EXPLORE and open the file ConnectingRod.top. 85

90 Type of constraint Origin Geometry Destination Geometry Axis on Axis Save the file. 9 Add the Piston Activate the assembly context menu then select Include sub assembly/part. Select EXPLORE and open the file Piston.top. Type of constraint Origin Geometry Destination Geometry Axis on axis Alignment on faces Save the file. 10 Dynamic Simulation First we need to tell TopSolid which parts need to move together. We do this by creating a Constraints system. Select Create Constraints system icon. 86

91 Select all the pieces to be involved with the simulation. - Shaft and Yoke. - Connecting rod. - Piston. - Arm. Use Esc to end the command. For correct simulation we also need to constrain the piston to the body. (Don t forget you will need to activate layer 1 to see the body simply left click on 1 on the quick layers tool bar). Select the Add constraints icon. Type of constraint Origin Geometry Destination Geometry Axis on axis NOTE: The connecting rod will automatically move to accommodate the constraints. You will be given an error at this point. This is expected. You now need to check your parts for correct design and alignment (Tip: Make the body transparent and view it from the side). Individual parts can be viewed or edited by using the modify element icon TEMPLATE. and then using 87

92 Add a blind nut from the AFNOR library (M8) onto the end of the shaft. You will need to use OTHER POSTITIONING. Place the nut down. Select ORIGIN GEOMETRY and proceed as before. To accurately simulate the dynamics (to make the nut rotate along with the shaft) we need to insert the nut into the constraints system we set up earlier. Open the tree and edit the constraints set, expand the constraints set and right-click on the components. Select Insert and click on the nut. Save the file. 11 Assembly Drawing Open a new draft document (A3 Horizontal mm). Select the Main View icon. 88

93 Select ASSEMBLY. Click in the model document. Use the view dialogue to configure the main view. Place it on the drawing and project a side view. Save the file. 12 Exploded View Go back to the model view (click on the title bar at the top of the window). Activate the Exploded view context menu. Click in the model document. Select a new design document then OK. Select OK. Click on the body. 89

94 The part will change color to green. Click onto the piston. Click on the connecting rod, then OK. Either type in a distance or just use your mouse.. Click onto the red torus to move it around, this defines the direction of displacement. Move it down to the shaft axis. Repeat the operation to explode the cover plate, screws, arm, shaft and yoke (all together) as shown here. 90

95 Then separate them as shown here: Select VALIDATE DEPENDENCE. 13 Add Exploded Axes (assembly lines) Select the Create Exploded Axis icon. Select AUTOMATIC. Save the file. Call it ExplodedValveAssembly. Switch back to the assembly drawing. We will now add the exploded view onto it. Use the Main view icon. 91

96 Select the exploded view model from the drop down list. Select MAIN ASSEMBLY and place the view onto the sheet. Save the drawing file and close the exploded model. 14 BOM & Indexes Activate the Bill of Material context menu then select. Choose the template called IdxNbDesMatCom.bom. Click in one of the 2D views. Click on the title block. Select the Automatic BOM Index icon. Click on the view you wish to place the indexes onto. 92

97 Save the file and close it. Design in place 1/2 Open a new design document. 15 The Hub Draw circle Ø200 at point 0,0. Extrude the circle by 100 along Z-. Draw a circle Ø150 at point 0,0. Use the boss icon create a boss 15mm high with the Ø 150mm circle. Place a 1x45 chamfer on the top edge. Define the part as Hub. 93

98 16 Plate Set layer 1 as current. Change color. Draw a Ø400 circle at point 0,0. Draw its axes. Switch off layer 0. Draw a circle Ø100 at the intersection point of the horizontal axis and the circle (200,0). Extrude the Ø 400 circle by 14mm along Z+. Cut a pocket through all with the Ø100 circle. Propagate the pocket through Z, 6 times through 360. Activate layer 0. Copy the edge of the boss on the hub to form a new circle. Cut a pocket through the plate using the circle. Switch off layer 0. Chamfer the pocket 1x45. Define the part: Plate. Place a new coordinate system on the face of the plate. Draw a circle of Ø175mm at point 0,0. Draw its axes. Add a M5x25 cap screw at one of the intersection points (87.5,0). Repeat the screw 6 times around Z. Use the screws process to drill the plate and tap the hub. 17 Spindle Turn the plate over and work on the underside. Make layer 2 current. Change colour. Draw 2 offset circles 15mm parallel to the existing circles as shown. 94

99 Create a point at the intersection of these 2 circles. Place a coordinate system on the point. Place a 8mm washer (ISO 7093) onto the point. Place a radial ball bearing (type AFNOR 20 02) on top of the washer (use then to pick a placing point on the top face of the washer and in the centre of the hole. Switch off layers 0 & 1. Move the washer and the bearing to layer 3. Draw a Ø8 circle at point 0,0. Extrude the Ø8 circle by 20mm (offset the extrusion by 2mm from the circle to allow for the washer). Draw a circle Ø20 at point 0,0. Create a boss 13.5mm high with the Ø20 circle. Draw a circle Ø25 at point 0,0. Create a boss 5mm high with the Ø25 circle. Add 1mmx45 chamfers. Define the part as: Spindle. Draw a horizontal line through 0,0 Cut a 2x2mm groove along the line. Add a thread to the Ø8. 95

100 Activate layer 1 (plate). Add a M8 tapped hole in the plate on the same point as the spindle. Make the absolute coordinate system current. Propagate the tapped hole; use a multiple propagation of a circular copy of 6 holes around Z and a simple mirror about the ZX plane. Place a blind nut on the spindle thread and propagate it (take the propagation from clicking onto the M8 holes). Use Repeat to do the same for the washer, spindle and bearing. Test your design by changing the Ø100 to Ø120. Define the assembly as carousel. 96

101 Do a drawing and BOM. Add a second drawing sheet with Tools, Drawing (copy the existing sheet and title block). Then add views of the separate components. Select the Main View icon (you now have 2 drawings so select the border of the new sheet) then use the assembly. to pick out the individual parts from Save the file. 97

102 98

103 Design in place 2/2 Topics covered: Contour Extrusion Assembly and design in place Most of the exercises performed to this point have been based on a single coordinate system: the absolute coordinate system. In this example, we will see how to use other types of coordinate systems. When there are multiple coordinate systems in the same file, it is essential to use the concept of the current coordinate system. The current coordinate system is the coordinate system in which the drafter will construct his geometry. 1 Contour Construct the contour by the point in the coordinate system. Comply with the dimension and the alignment constraints Position the part in relation to the absolute coordinate system so that its origin is on point 1. In doing so, the position of the contour is constrained, and therefore a dimension must be created

104 Note: For a dynamic displacement, use the Move parents function. The NON-DYNAMIC option is used for displacement between two points. Draw a line by two points and create the dimension To make the Oblong profile, use the Thicken operation on the line. Select the SYMMETRICAL OPTION = YES with a thickness of 2mm; the end is the inner arc type Replicate the oblong profile by translation along the Y- axis of 25mm Note: Any replica element is exactly identical to its original. 2 Extrusion By selection, extrude the contour as well as the two oblong profiles on 4mm along the Z+ axes. Note: By clicking on the red arrow, the extrusion direction is reversed

105 3 Creating a coordinate system on the lower face of the plate. To create a coordinate system on a face, it simply needs to be made current. Name the coordinate system F2. After increasing the extent of the coordinate system using Modify element, draw a RECTANGULAR contour. Dimension the contour as shown to the right. 4mm extrusion of the contour along the Z+ axes. Creating a contour on the face at a 30 angle. Dimensioning of the contour in relation to the edges of the plate. 101

106 Extrude the contour 8mm along the Z- axis. Make the two 5mm fillets. Subtract the solid from the plate then make two Ø3mm drill holes concentric to the 5mm radii. Drill at M4 and repeat the drilling in each corner. Note: Use the edges of the plate to indicate the two propagation directions. Make current the 2 coordinate system. Duplicate this coordinate system by translation along Z+. To indicate the displacement value, specify the plate with the 4 holes. Name this new coordinate system 3 and make it current. Draw a RECTANGULAR contour. Dimension it to have a 2mm margin on all sides. Execute a 25mm extrusion. 102

107 Modify the M4 tappings and replace them with Ø4.5 holes. Call up the standard component library and take a CHC M4x16 screw. Position it on the coordinate system of the first drill hole and repeat this using the 4-corner drill hole propagation. Execute the TAPPING procedure on the lower block, specifying which face to drill. Save the file. Use the Assembly, Part definition function to attribute a designation and characteristics to each of the parts. Click the parts, validate and fill in the boxes according to the values: Designation: Plate Reference: P01 Also attribute a designation to the assembly. 4 Creating a part to assemble Open a new Design document. Create the insert shown here. Start by drawing a rectangular contour of 41.5mm x 8mm, to which you apply 2 fillets of radius 5mm. Construct a 3mm parallel. Extrude this parallel by 2.5mm, then add a boss with a height of 2mm. Save the file and remember to use the Part definition function. 5 Assembly Open the document containing the in situ assembly. Import the last part created using the Assembly, Include assembly/part function. Place the insert in the Assembly document by clicking a point anywhere in the workspace. 103

108 Show a face of the insert and make it correlate to the bearing face on the square. Validate the contact distance. Continue, specifying the next faces in order to position the insert in the notch on the square. 6 Layout Call a new Draft document. To create the layout of an assembly, you need to select the Main view function click on the ASSEMBLY button. and then must If the 3D document is open, you may then select it by clicking directly in the document or via the dropdown list; otherwise, you have to use the BROWSE button. Select the desired view configuration and place it in the drawing. Create the desired auxiliary views. To insert a bill of material, use the Bill of material function, select the IdxNbDesMatObs table model, click the ASSEMBLY button and select the assembly file name in the drop-down list. Select Depth=FLAT LEVEL and click the title block to position the table. 104

109 Then show the parts on the views to position the coordinate systems. Regenerate the bill of materials using the function. 105

110 106

111 Components 107

112 Concepts to introduce: Define the geometry Define the drivers Define the tools associated with the component Define the key points Edit the component's catalog Save a standard template 1 Define the geometry Create a new Design document. Tools, Coordinate System menu. Select XZ. Select SET AS CURRENT. Select TOP VIEW. Enable the Curve context. Then create the contour representing the half-part. Dimensioning the contour: linear dimensioning and half-part dimensioning for diameter dimensions. Adjust and name the dimensions. Enter a name for each of the driver dimensions. Name di = inner diameter Name ht = height of the collar Name h = height of the body 2 Adjust the dimensions Modify the dimension to di+5 for the body. Modify the dimension to di+10 for the collar. 108

113 Enable the Shape context and create a revolution shape. Create the chamfers from 1 to Define the part Assembly context, Define part. Click on the part, enter the part characteristics: designation, reference, material, etc. then OK. Save the document as Ring. 4 Define the component Assembly, Define Component menu. Note: Cut the Define component menu to keep it open. 5 Define drivers Assembly, Define Component, Define drivers menu. Click on dimension di. Enter the driver designation: Inner Diameter, then OK. Note: A set of drivers is created. Repeat the operation for the other drivers, ht and hc: Body Height for hc, Collar Height for ht. 6 Define the key points The key points are the component positioning points. In our example, we are going to define two positioning points, below and above the collar. Set the absolute reference on current. Assembly, Define Component, Define key points menu. Click on the absolute reference. Erase ABSOLUTE REFERENCE and enter BOTTOM, then OK. Note: A set of key points/references is created. Create a duplicate coordinate system. Click on the absolute reference (current reference). Select TRANSLATION. 109

114 Select Z+. Enter parameter ht (height of the collar). Click on the newly created reference. Enter TOP, then Enter. Select OK. 7 Insert the part into an assembly Open or create a new Design document. Select Ring in the list of open components. Enter the required values: di = 20mm hc = 10mm ht = 10mm Note: The proposed values are the template values. Click on the position of the component on the receiving part. Note: The positioning of the component is defined by a reference positioning on a reference on face with constraints. Select STOP. The component is positioned in relation to the first key point. Select as required, then STOP. Bottom Top 110 Save the assembly document, then close. 8 Define the tools If required, go back to the Ring document.

115 Display the ring control elements. Set the sketch reference to current. Select REFERENCE ELEMENT. Click on the sketch. The sketch creation reference becomes current. Set level 1 on current. Click on the knurled wheel on level 1. 9 Create the tool geometry as the ring geometry Adjust and modify the dimensions according to the parameters. Deactivate level 0. Create a revolved shape. Modify the tool transparency if need be (transparency attribute). Assembly, Define component, Define tools menu. Select SUBTRACT OPERATIONS ON SHAPES, then click on the tool shape. Enter the tool name: Ring housing. Enter the tool designation, then OK. Note: A set of tools is created. Save the document. Open the previous assembly document. Enable the Assembly context and select Use processes. Click the Ring. 111

116 Click the shape which is to undergo the process. Select STOP. Note: The process associated with the ring is displayed in the alpha bar. If need be, use the modification of the positioning in order to change key points. Save the document. 10 Edit the component's catalog Return to the Ring document. Assembly, Define Component, Edit catalog heading menu. Select All the parameters and texts. Note: Excel starts automatically if it is installed on your station. If it is not, Windows WordPad is opened. Enter the various values for your rings. Save the Ring.xls file. Quit Excel. 11 Test the catalog Assembly context, Catalog code. Select the code of your choice. Open the assembly document. Modify element. Click the ring. 112

117 Modify the code. 12 Save a standard template Assembly, Define Component, Edit/save template. Select SAVE STANDARD TEMPLATE. Enter your component s classification. 1. Select Standard MY 3D STANDARD 2. New Family GUIDE 3. New Type RING 4. New Variant COLLAR 5. Keep version Keep Representation NORMAL Select OK to validate. Note: The part file is RING#V=COLLAR#I=00#R=NR.top #V corresponds to the variant. #I corresponds to the version. #R corresponds to the representation. 7 Edit the standard component's catalog Assembly, Define Component, Edit catalog heading menu. Select All the parameters and texts. Enter the values or copy / paste the values from the previous catalog. Save the file. Quit Excel. Note: The Excel file is name of template file.xls, In this case = RING#V=COLLAR#I=00#R=NR.xls. 8 Create a picture File, Save as menu. Select the Bitmap format, then OK. Adjust the values, then OK: Size Type Background color 300x300 PNG WHITE Click anywhere in the view to be captured. Note: The BOX option is used to frame part of the view. Close the file. 113

118 9 Use Open or create a new Design document. Enable the Assembly context and select Include standard. Select MY 3D STANDARD, then GUIDE. 114

119 Kinematics & Dynamics 115

120 Kinematics Concepts to introduce: Joints. Scenario. Trajectory. Replicate a state. Positions. Rigid sets. Check collisions. Approach. Introduction The kinematics menu is used to define and simulate an articulated mechanism. It is possible to define kinematics after the event on a predefined mechanical assembly. It is possible to define kinematics for a mechanical assembly that includes parts made in place (kinematics is independent of positioning constraints). It is possible to define kinematics for a wireframe model in order to complete a preliminary study. It is possible to define several scenarios for the same kinematics, in order to study several phases of the movement. It is possible to define stops on joints. A few complex joints are available in order to represent, for instance, the screw / nut systems and gears. It is possible to generate a video clip of the graphical animation for marketing purposes. Principle: The definition of the mechanism s kinematics is done using two types of elements: Joints Joints enable us to define mechanical articulations between elements. A joint is defined between a base element and a linked element: When the joint is enabled, the linked element moves in relation to the base element, which remains fixed (unless it is itself a linked element in another joint, or attached to a linked element). It should be noted that a joint is always defined between two simple elements. For instance, when a joint is defined between two sub-assembly components, it is defined between two simple elements in each component. In contrast, when defining a rigid set, when we designate a composite element (sub-assembly component, group), all its parts are assumed to be rigid. It is nonetheless possible to make the elements of a single component mobile in relation to each other, by using the designation with detection (as this is less practical, it is recommended to organize the design of the mechanism in non-articulated subassemblies). Kinematics defined in this way are used to perform various simulations: animation, trajectory analysis..., but to do this, it is necessary to define the phase of the movement to be simulated, using a scenario. A scenario is a text file associated with the document (filename extension.scn), which describes the evolution of the articulated driving coordinates in the form of a simple column-based table, whose first column specifies the date when the articulations are performed, while the subsequent columns specify the values for the articulated coordinates at this date. There may be several scenarios for a single kinematics (each scenario being identified by a name), which will help to study several phases of the movement. Rigid sets Rigid sets allow us to group together moving rigid elements in a logical manner (by default, each element is assumed to be free and independent). The elements in a single rigid set are considered to be immobile in respect of each other, such as, for instance, parts fixed by screws or bolts. 116

121 These sets are grouped together in the rigid set group, which can be edited in the symbolic tree. It should be noted that there is no point in defining rigid sets when setting up a kinematics on a simple set (pre-study) where each element is independent. Steps: To begin a study, follow these steps: Model the mechanism in one of its kinematic states, using the standard functions. If necessary, define the rigid sets. Define the kinematic joints. Create a scenario. Launch an animation, in order to view the movement. The kinematics definition being associative, it is obviously possible to modify the mechanical assembly and to restart a simulation directly. 1 Joints Open the Kinematics document. Study of a hand pump mechanism. Enable the Kinematics context, then select Joints. 2 Chassis Select FIXED. Click on the absolute reference. The tree opens automatically to display all the joints. NOTE: A set of joints is created. 3 1 st joint Select PIVOT. Click on the chassis (absolute reference). Click the handle. Click the X- rotation axis of the handle in relation to the chassis. Select OK. 117

122 Name the joint: A. 4 2 nd joint Select PIVOT. Click the handle. Click the connecting rod. Click the rotation axis X- of the connecting rod in relation to the handle. Select OK. Select ANONYMOUS. 5 3 rd joint Select PIVOT. Click the connecting rod. Click the piston. Click the rotation axis X- of the connecting rod in relation to the piston. Select OK. Select ANONYMOUS. 118

123 6 Last joint Select PRISMATIC. Click the chassis. Click the piston. Click the piston axis. Select OK. Select ANONYMOUS. 7 Scenario Enter the name of the scenario CYCLE in the New scenario area, then select OK. Enter the scenario: rotation angle of the handle according to time. Select ANIMATE. Click on to launch the simulation. NOTE: it is possible to create as many scenarios as required. 8 Trajectory Calculation Create the connecting rod middle point Select Trajectory 119

124 Select FIXED COORDINATE SYSTEM. Click the connecting rod. Click the point. 9 Replicate a state Select Replicate a state. Enter the time and level of the element to be replicated: time = 2 and level = 5, then click the connecting rod. 10 Positions Select Positions. Select FIXED COORDINATE SYSTEM. Click the connecting rod. Click the connecting rod. Some positions overlap. 120

125 11 Rigid sets Create a cylinder with a 20 mm diameter. Select Rigid sets. Click the piston sketch. Click the cylinder, then STOP. Note: a set of rigid sets is created. Each rigid set contains elements which will move together during the simulation. 12 Check collisions Used to check collisions during the movement. Only works on 3D templates. Enable level 1.. Select Collision Control Set. Enter CHECK1. Click the cylinder. Click the ring. Note: a set of collision checks is created. Select Animate. Check Stop when collision box. Select CHECK1. Check Stop when collision. Launch the animation. Note: The simulation will be interrupted on the first collision encountered. Select Duplicate state to keep the parts in collisions. 121

126 Enter Level = 3 and click the cylinder. Note: a set of sets of kinematic shots is created. Each set contains the mobile elements involved in the simulation. The time is indicated in the group name = second in the CYCLE scenario. 13 Approach Used to calculate the distance between two bodies during the simulation. Create an extrusion of the sketch of the 10 mm handle in CEN- TERED mode. Create a rigid set comprising the sketch and the shape. Select Closest approach. Click the cylinder. Click the new handle shape. Click on OK. The approach lines are displayed on the screen. The approach distance is displayed in the alpha area: Approach distance = [61.181mm, mm] NOTE: it is not possible to display the simulation and the lines or to adjust the number of lines. A nil approach distance indicates a collision. 14 Stops Edit the set of joints. Right-click on the pivot joint: A. Select Modify in the context-sensitive menu. Select NO INITIAL VALUE. Select NO MINIMUM VALUE. Enter 30 as maximal value. Launch the simulation. The Stop exceeded (A) message is displayed in the alpha area. This is because the max. A value is reached, whereas in the scenario the A simulation angle is 45. The state can be replicated if required. 15 Application on parts Open the Assembly file. Add the joints. 122

127 Simulate the movement. 123

128 Dynamics NOTE: Dynamics only works on an assembly with a constraint system. Concepts to introduce: Gravity. Animate. Measurement. Record measurements. Export and analyze results. Open the Pump file. 16 Gravity Select Add Gravity. Select OK. Select Z- or click on the cylindrical face of the body of the pump. Gravity is represented by a red arrow. NOTE: A set of forces is created, and gravity is to be added to this set. 17 Mechanism calculation Select Animate. Select to launch the calculation. Select to launch the simulation. Move the absorption factor and observe the difference. Select to launch the calculation. Modify the physical attributes of the handle and change the material: aluminum. Select to launch the calculation. 18 Measurement We wish to measure the angle between the connecting rod and the body of the pump. 124

129 Select Measure. Select the ANGLE measurement type and enter a name for this measurement: MEASUREMENT1. Click Z- or the pump axis. Click an edge of the connecting rod. Select OK. Select NEW MEASURE SET. Enter the name of the measurement group ANALYSIS. NOTE: A set of measurements is created, and the angle measurement is to be added to this set. 19 Record measurements Select Animate. Select to access the options. Check Measure and select ANALYSIS. Select Browse, then specify the file name and location. Note: file name_measurement name.xt is proposed as the file name. You can select an.xls extension. In our example PUMP_ANALYSIS.XLS, since we are going to plot the curve with Excel. Select to launch the simulation. Close the animation box. Open the PUMP_ANALYSIS.XLS file. Plot the curve. 125

130 126

131 Surfaces 127

132 Topics covered: Basic surface design (Loft, Offset, Flat...) Advanced design (Dome, Blend, Swept...) Surfaces operations (Remove, Sew,...) 1 Contour creation Create a new Design document. Select Tools, Coordinate System. Select XZ. Select SET AS CURRENT. Select TOP VIEW. Select Edit, Name. Click on the coordinate system. Input FRONT, then OK. Set layer 1 as current. Select Curves context, create a line from 0,0 to 0,150. Select Curves context, create 2 points on the line, then dimension them like here. 128

133 Select, then ABSOLUTE COORDINATE SYS- TEM. Switch to a perspective view. Create coordinate systems to create section curves. with Tools, Coordinate System. Click on previously created points. 2 Create section curves Create a circle, diameter 60mm, centered on the absolute coordinate system. SET AS CURRENT the second coordinate system. Create an ellipse, center 0,0, X Radius=30, Y Radius=25 SET AS CURRENT the third coordinate system. Create a circle, diameter 50mm, centered on the current coordinate system. SET AS CURRENT the fourth coordinate system. Create a circle, diameter 25mm, centered on the current coordinate system. Set the line invisible. 3 Loft Surface Select Loft surface. Select curves. 129

134 All curves are in the same direction. Select STOP WITH NULL CURVATURE. Create a 45 sketch line through the point 0,50., passing Create a 5mm offset line. Shape, Trim Select BY SWEEPING CURVE, then click on the surface. Click the 45 sketch line. Select KEEP BOTH PARTS. Change the color of the top surface. 4 Offset a surface Shape, Other Operations, Offset Click on the top surface. Global distance = -2mm. Select SAME DISTANCE FOR ALL FACES. Trim the surface by the offset sketch line. 130

135 5 Ruled surface Ruled Surface. SET AS CURRENT the absolute coordinate system. Switch to a perspective view. Click on boundaries of the 2 surfaces, invert direction if needed. 6 Create the top of the bottle SET AS CURRENT the highest coordinate system. Create a duplicated coordinate system on Z+ = 2mm. SET AS CURRENT the new coordinate system. Create a circle current coordinate system., diameter 25mm, centered on the Extrude, SURFACIC on 15mm. 131

136 Ruled surface Click both edges as show on the bitmap. Result. 7 Create the bottom Set as current Layer 2. SET AS CURRENT the absolute coordinate system. Create an Ellipse on 0,0, X Radius = 25 and Y Radius = 20. Create axis on the ellipse. 8 Flat surface Copy edge from the loft surface. Copy Edge. Click on the boundary of the loft surface. 132

137 Switch off layer 1. Flat surface. Select the 2 curves, then click on OK. 9 Dome surface Driving elements. Click on the flat surface. Create intersection points between the ellipse and its axis. SET AS CURRENT the coordinate named FRONT. Create a circle. Create two arcs passing by 3 points like shown below. Trim both arcs on their intersection point Create a dome. Click on the ellipse. Click on the first arc. Click on the second arc, then OK. An axis has been automatically created. Select OK. Select OK. 133

138 10 Blend surface, 3 faces Select Transparency = 6 then click on the body of the bottle. Create Blend. Select 3 FACES BLEND. Click on the body of the bottle. If needed, invert the direction, then select OK. Click on the flat face. If needed, invert the direction, then Select OK. Click on the dome surface. If needed, invert the direction, then select OK. Click on the circular edge. Result. Set the flat surface on layer number

139 11 Trim surfaces Select Trim. Select BY IMPRINTING CURVES, then click on the body of the bottle. Click on the edge of the 3 faces blend surface. The arrow shows the side you want to remove, then, click on OK. Click on OK. Select NO then OK. Repeat the operation with the dome surface. 12 Create the thread SET AS CURRENT the highest coordinate system. Set current layer 3. Create a duplicated coordinate system on Z+ = 5mm. 135

140 Select Curve, Other Curves, Spiral / Helix. Click on the 0,0 point. Input values like shown on the bitmap, then OK. 2mm. Create a rectangle, CENTERED, X = 2mm and Y = Swept surface. Select the first choice: One guide curve and one section curve. Click on the helix. Click on Z+. Select POSITION SECTION CURVE. Click on the rectangle. Select USE CURRENT COORDINATE SYSTEM ORIGIN. Click on SURFACE to switch into a SOLID mode, then OK. Create fillets of 5mm. 136

141 Create chamfers 0.75mm x 0.75mm. 13 Remove face Remove the internal face of the thread. Remove. Click the internal face like shown. Select OK. Duplicate the thread with a 180 rotation around Z+. 14 Intersection of faces Intersection Click on the top of the bottle. Select ALL FACES. Click on the thread. Do the same thing for the second thread. 15 Imprint Imprint. Click on the top of the bottle. Select all curves we've created just before. Select NORMAL. Select OK. Remove imprinted faces on the top of the bottle. 137

142 Create a circle, diameter = 25mm, on point 0,0. Trim the 2 threads by this circle. 16 Sew surfaces Sew. Select all surfaces. Select DON'T COPY BOUNDARY EDGES. NOTE: You've a message in the alpha bar: Result is a surface. 17 Thicken Shape, Other Operations, Thicken. Input 0.5mm along the arrow direction, then OK. Result. 138

143 Mechanically Welded Chassis 139

144 Concepts to introduce: Assembly on a sketch. Constrained assembly. Modifications. Cuts. 1 Assembly on a sketch Open the ChassisSketch document. In the Assembly context, click on. Select a 200 UAP beam extruded. Click on the 1 st point in the segment. 1 Click on the 2 nd point in the segment. If need be, turn the iron by entering an angular value (90 or 180 ), then click on STOP. Repeat the procedure on the other extruded elements

145 Note: In this example, in order to avoid having to enter an angular value, click on the points counterclockwise. 2 Curve trimming: Miter cut In the Shape context, click on. Scroll down the list and select EXTENDED CUT, then in Mode, select MITER CUT. Click the first shape. Click the second shape. The arrows indicate the cutting direction for the extruded elements. 1 Click on OK. Result of the cut. 2 Repeat the procedure on the other extruded elements. 141

146 Lay the crosspieces in the same way as above. 3 Curve trimming: Main cut 1 In the Shape context, click on. Scroll down the list and select EXTENDED CUT, then in Mode, select MAIN CUT. Click the first shape. Click the second shape. The arrow indicates the cutting direction for the extruded element

147 Result of the cut. Click on OK. Repeat the procedure on the other side of the extruded element, then on the other crosspiece. 4 Changing the orientation In the system bar, click on Modify element the1st crosspiece., then select Click on POSITIONING. Enter 180 in the rotation angle area, then click on STOP. Result of the change in orientation. Repeat the procedure on the other crosspiece. 5 Assembly on sketch and face In the Assembly context, click on. Select a 100x10 equal-sided Angle Extruded Rolled. Select the axis. Click on OK. Select the outer face of the 1 st curve. Select the outer face of the 2 nd curve. 1st face 2nd face Rotation angle = 180. Scroll down the key points by clicking on CORNER POINT until the result below is obtained, then STOP. 143

148 Assembly result. Repeat the procedure on the other crosspiece. 6 Assembly on point and face In the Assembly context, click on. Select a 50 U-shaped Small Iron Extruded Rolled. Click on THROUGH POINT. In the system bar, click on, then in the point bar, click on point on curve. Select the edge of the crosspiece. Click on Y-. Rotation angle = - 90, then STOP. In the Curve context, click on Dimension. 144

149 Click on the point, then on the edge, and adjust the dimension to 300mm. 7 Constrained assembly Beam 1 Assembly In the Assembly context, click on. Select a 200 UAP Poutrelle extruded. Select CONSTRAINED POSITIONING. Enter 1000mm. Select OTHER POSITIONING. Click in the graphic area to position the component. Set the assembly constraints as follows: - Mate at extremity of extruded element on blue face. - Alignment of green faces. - Alignment of yellow faces. 8 Beam 2 Assembly Repeat the procedure for the following extruded element: extruded element length = 500mm. Set the assembly constraints as follows: - Mate at extremity of extruded element on green face. - Alignment of blue faces. - Alignment of yellow faces. 145

150 9 Modification of key point Lay a 50x5 equal-sided Angle extruded as shown below. Perform the trimming operations. 10 Change the 1st point Open the construction tree and edit the extruded element. Click the right mouse button to display the context-sensitive menu, then select Replace. 2 In the list of points, select the half-way point of the extruded element. 1 NOTE: you can either use the center point of the edge or the point on curve option in the drop-down list. by selecting the middle Perform a PLANE SYMMETRY repetition along the ZX plane of beam 1 and 2 and of the brace. 146

151 11 Do a Chassis assembly layout Set the bill of materials for material use. 147

152 148

153 Sheet Metal Work & Piping 149

154 Concepts to introduce: Assembly on a sketch. Inserting components. Creating a pipe line. Processes. Creating a plate. 3D contour. 3D dimensioning. Pipe line layout. 1 Assembly on a sketch Create the following sketch at level 0. Enable level 1. Include an AFNOR Boilermaking, Tank, Collar = Ø800, thickness = 10 between the two points on the horizontal sketch. 150

155 Include an AFNOR, Boilermaking, Bottoms, Dished bottom for pipes, Ø800x10 on curve and point reference. Set level 2 to current. Include a TOPPIPING Stainless steel, Accessory, Welding neck flange = PN10 DN200. Select the coordinate system on point. Click the upper vertical curve. Note: you can select the curve to automatically position the usual flange for the curve, and then merge the created point with the end point of the curve using Edit, Merge. Repeat the procedure for the lower curve: positioning of the flange and point merging. 151

156 Note: You can use Copy component to include the same component. 2 Create a pipe line In the Piping menu, select Create a pipe line. Click the upper vertical curve. Click the flange. Select STOP. Adjust the parameters, then OK. 152

157 Repeat the procedure for the lower curve. 3 Processes Select Processes. Click the tube. Select Outer branching, then click on the ferrule. Select STOP. Click the ferrule. Select inner trimming, then click the tube. Select STOP. Repeat the procedure for the bottom tube. Set level 3 to current. Create a point on the horizontal sketch, 100mm away from the left extremity with Point on curve. Dimension the point and adjust the dimension to 125mm. Create a reference on point. Turn the reference around X to switch to plane XZ / absolute reference. 153

158 Deactivate levels 0,1 and 2. Create a U-shaped curve centered on X. Create a 620mm extrusion along Z-. Create a YZ plane. Create a circle with Ø812. Create two sketches at 30 and -30. Create two parallel lines at 50mm. Trim the circle using the parallel lines. Create a 250mm extrusion with the arc, leaving the sketches visible and using a 25 offset. Create a trim on the U with the arc. 154

159 Enable the Sheet metal context and select Create Sheet Metal. Click the lining. Enter thickness = 12mm and reverse the direction if need be. The direction of the lining thickness is towards the ferrule. 4 Create 8-size fillets on the U Create a plate on the U, 8mm thick, with the direction of the material towards the outside. 155

160 Create a plane on the planar face of the U. Create a 740 x 200 rectangular contour. Create a point in the middle of the long edge of the U. Dimension, constraint and adjust the dimensions as shown in the picture below. Create a 12mm extrusion. Create two holes with Ø22 as shown. Enable the other levels. Set the absolute reference as current. Create a repetition along YZ of the foot. 5 3D contour Open the InstallationWithout pipes. Deactivate levels 2 and 3. Assemble clamps PN16-DN100 on the Tank and Tank3. Select 3D Contour. Select CURRENT COORDINATE SYS- TEM. Click a flange. 156

161 Click the flange reference. Select >>. Set the REFERENCE PROTRACTOR on 90, then OK. Move the mouse to the left and enter 500mm. Move the mouse up and enter 500mm. Select WIZARDS. Select CUBE. Select the point in the center of the TANK3 flange. Using OTHER WAY, select the right line, then OK. Select STOP. In the Piping menu, select Create a pipe line. Click the 3D contour. Click the flange. Click the other flange, then select STOP. Adjust the parameters, then OK. 6 3D dimensioning Select 3D dimensioning. Select AUTOMATIC DIMENSIONING. Click the 3D contour, then QUIT. 157

162 Delete the dimension and adjust the dimension from 500 to 200mm. 7 Pipe line layout Select Main view or. Select ABSOLUTE COORDINATE SYS- TEM. Click on the pipe line in the 3D template. Place the view. 158

163 8 Piping dimensioning Select Piping dimensioning. Click the elbow. Click the other elbow. The dimension is displayed in dynamic mode. It is also possible to change its orientation by selecting the MEASUREMENT button, and then setting the dimension. 159

164 160

165 Realistic Rendering 161

166 Concept to introduce: Use advanced functions of imaging Add, replace and adjust texture layers Add reflections and relief Manage lights and textures Set conical views Activate advanced shadows Set up anti-aliasing Use shaders and advanced renders Insert logos 1 Open the document Bank.top 2 Shift to realistic rendering 3 Click the icon Display If the TopSolid/Image icon bar is not visible, display it by right-clicking the menu, and selecting Image. 4 Click the view The image displays throughout the progress of the calculation. The colors and textures are similar, but the lights are of much higher quality. In order to cover the windows, we wish to replace their plain green color with a texture. 5 Click the Textures icon, and select the left green window 6 Click the Textures radio button Add a layer using the Add layer button. In the Pattern tab, select the Plastics family. Click the blue texture in the top left corner. When TopSolid Image is installed, the Apply button previews the result in realistic rendering, and the Preview button previews the result in Image rendering. 7 Click OK The green color on the left window is replaced with the blue texture. To apply the same texture as the right window, just copy the material (transporting the texture information) from the left to the right window. 162

167 8 Run Attribute, Material Click the left window to define the template, then the right window to indicate the part to modify. 9 Restart a TopSolid Image rendering The scene is lit (among others) by a spotlight located above the teller. We now light it from the front. 10 Click the Light icon The light configuration box displays. 11 Modify the spotlight parameters Select the Spotlight above spotlight. Disable it by unchecking On. Select the Front spotlight, and enable it by checking On. 12 Click the Apply button to view the new configuration, then click OK 13 Restart a TopSolid Image rendering The shades projected by the spotlight are neat, with a sharp edge. 163

168 14 Modifying the shades In order to soften their outline, open the light box, select Front spotlight, and position the Shade diffusion cursor on the 4th position. Restart a TopSolid Image rendering to observe the variation. Now save an image of the project. 15 Save the image in a file Click the Save icon. Click the view. Keep the name and format proposed (bank.jpg). Enter the size required, and click OK. The image is calculated, then saved. Managing the environment Creating a frame 16 Load the file Case.top In order to produce more relief, we wish to view the case with its shade projected onto the ground. 17 Create a mark on one of the case s feet in the horizontal plane In this work plane, create a large rectangular flat surface. Considering the perspective, we can plan a surface 5 to 10 times larger than the subject. 18 Zoom in on the object while orienting the view approximately according to the result required 19 Allocate a floor board texture to the surface, and set the scale in the Parameterization tab We recommend setting the dynamic rotation centered around the subject. 164

169 Adjusting the lights To enhance the subject, light it using a spotlight lighting it exclusively. To ensure easy lights adjusting, shift to 4 views, with the perspective view close to the result required, and the other views sufficiently far away from the subject to contain the lights. 20 Creating new light Open the lights configuration box and deactivate directional light. Create a new light of the spotlight type. Set the origin of the spotlight in the top left corner and in front of the case. Adjust the spotlight s opening in order to light only the subject s surroundings. To use dynamic lights adjusting in the views, we recommend reducing the project s window, and moving the lights configuration box outside. In the realistic rendering, the ground seems black. This is due to the fact that in accelerated rendering, only the tops of the polygons are lit. In the case of the ground, its 4 corners are outside the spotlight zone. 21 Adjusting the tolerance In the status bar, click the Tol zone, and activate the Max facet size zone. Set the value to 200mm. 165

170 The ground is now cut into 200m long triangles, which can be lit properly. Please note that this procedure is required only in accelerated rendering. TopSolid Image calculates the image properly without this additional cutting. Adjusting the camera We now adjust the camera into the conical perspective mode. This mode is more realistic than the parallel perspective used in design. 22 Shift into the on conical perspective view mode Zoom in on element on the case. Turn around the part to position it vertically with the spotlight to the left and the lighting mark on the ground to the right. Open the camera configuration box. 23 Select the Parameters tab, and click the view Select the conical projection and choose a 35 viewing angle. Click the Longitude, latitude, radius mode, and set the 3rd parameter to the value 800 (this parameter corresponds to the distance between the camera and the point targeted). Click OK to update the view. For information, the human eye has a viewing angle ranging from 35 to Click QUIT, then rotate and translate the part until the scene is satisfactory. Launch a rendering using TopSolid/Image. You can save the camera s status using save view s configuration. It can be interesting to rotate the ground s texture (Rotation field in the Parameterization tab) to prevent the patterns from being too well aligned with the case of the viewing direction. Adjusting shades The shades obtained are a little too sharp. They can be softened. 25 Open the lights configuration box, select the spotlight, and set the Shade diffusion cursor on the 3rd setting The shade projected by the subject is softer. 26 Open the lights configuration box, select the spotlight, and define the Penumbral shadow half-angle field to 10 The spotlight s bright-dark transition zone is now larger. 166

171 Managing materials Colors 27 Load the Drill.top file The first step consists in coloring the assembly. 28 Modify the rear part s texture, and select a yellow ambient and diffuse color yellow. Also, color the front part in green. Colors and textures can be easily copied from the front part on its symmetry using the Attribute, Material function. 29 Turn the part slightly facing you, and apply a TopSolid Image rendering. We now wish to have an aspect slightly lighter on the front part. 30 Modify the texture on the front part: set Smooth aspect to 20 and Brightness to 50 Basic textures Layers Textures are defined by a superimposition of layers which each provide their own effect. Certain effects are integrated into a same layer. 31 Load the Vase.top file Add a texture layer with a pattern Minerals, Pink granite. The rendering is rather dull. Adding a brightness effect is required. 32 In the Colors page, set Smooth aspect to 20 and Brightness to 50 In the Textures page, Style tab, check Specular. The Specular option enables adding the specularity effect to the color effect provided by the texture. However, for a more advanced reflection effect, we can use a special layer. 33 Add a texture layer, select the Reflections / Brightness pattern, and choose the Reflection effect parameterization We then use this effect added to the basic pattern. 34 Modify the 2nd layer, by shifting its style to Add with a value

172 Style In the previous exercise, we used the Add mode. 35 Try the Add, Mix and Filter modes The types of plating enable using an existing texture with other colors. 36 Delete the second layer, and replace the current pattern by Textile/Spotted fur 37 Select the Degraded type, and define the first color with a light color, and the second color with dark brown. Parameterization The parameterization tab enables choosing a texture plating adapted to the object s shape. 38 Load the Vase.top file and add a layer of the TopSolid/Marble texture The texture is tightened on the level of the collars. 39 Set the parameterization to Auto axes The texture is less distorted, but the texture seams are visible. 40 Set the parameterization to Cylindrical, click Main mark, and set the values U Scale to 0.2rev and V Scale to 50mm The result is correct, except on the level of the foot, which is too horizontal. TopSolid Image s 3D textures do not need 2D plating, and do not suffer from any distortion or seam effect. 168

173 TopSolid Image textures Pattern 41 Replace the Marble texture by a Light- Works/STONE/Marble texture, create a new instance with a 10mm scale As the texture is defined in 3D, there is no distortion. 42 Create in a new file a RECTANGULAR extruded (wood powder). Add a texture with a LightWorks/WOOD/Wood pattern Please note the continuity of the texture between the faces. Displacement 43 Test the various shaders available Reflectivity The mirror shader enables simulating a quasi-total reflection effect, as a mirror does. The metal shader enables simulating a metallic aspect, with reflections. This shader is different from the others, as it also impacts the part s color. The glass shader enables simulating reflection and refraction effects specific to glass materials. 44 Open the Chest.top file 45 Include the Vase.top file on the furniture. Modify the vase, in order to ensure its attributes are piloted by the component, then select a glass texture. The glass aspect is better when the scene is surrounded with an environment enhancing the reflection effects. 169

174 Advanced rendering Study of a metallic part 46 Open the Holder.top file and perform a rendering The result lacks brightness. 47 Modifying the part s texture Increase the smooth aspect to 20 and brightness to 50. The rounded edges are brighter, but overall it remains dull. 48 Modify the part s reflectivity Add a layer of reflectivity of the metal type, and choose aluminum. The result is correct, but the clear shades do not provide a pleasant result. 49 Modify the shades Open the lights configuration box, select the front light and set the Shade diffusion cursor to the third setting. The result is clearly more pleasant for the eye. 50 Modify the texture Choose gold, copper, etc. Play on the various shade parameters. We now want to give a more irregular aspect to the surface. 51 Modify the part s texture Uncheck the shader for reflectivity and select the pattern Metals/Rough galvanized metal sheet. Add a new layer. Use the Add style with a value 1, and use the reflectivity shader defined previously. Change it by setting the values Ambient factor and Diffusion factor to zero. The result combines the pattern of the first layer with the reflection of the second. We can note that the part has bluish reflections. This is due to the reflection of the screen background in the part. We can avoid this effect, by changing the application s background color to black. But in this case, the image obtained will have a black background if the background is visible in certain locations. In order to achieve a rough aspect, a displacement shader is added. 170

175 52 Modifying the part s texture Add to the first layer a rough displacement shader with a 20mm scale and a 0.1 amplitude. We obtain a rough aspect, but it is too strong to enable the reflection to provide an effect. 53 Modifying the amplitude of the displacement shader to 0.02, and the metal layer reflection factor to 0.3. We obtain a reflection distorted by the perfectly realistic roughness. Managing textures and logos 54 Load the Case.top file. We wish to add a logo in the hollow section of the case. 55 Modify the texture of the blue panel on the front of the case Add a layer, and choose a logo on a white background in the TopSolid Logos family. In the Parameterization tab, choose the Orthographic type and uncheck Wrap U and Wrap V. Uncouple the U and V scales, and set the U scale to 100mm and the V scale to 50mm. Center the logo approximately. In the Style tab, choose the Relief mode, and set the value to 2. Realistic display becomes very slow. The relief display can be deactivated in the rendering viewing options (Relief, Viewing option).the TopSolid Image rendering takes the logo into account in relief. We now wish to replace the TopSolid logo with a personal Missler logo. 56 Run the Attribute, Texture function, and click MANAGING TEXTURES. 171

176 57 Create a new family Click Create a new family and create a family named My logos. Then click Import texture and select the Missler.gif file. In the texture definition box, check the Logo option, then click OK. This bitmap can now be used as a texture by TopSolid. 58 Replace the TopSolid texture by the Missler texture in the My logos family, and run a TopSolid Image calculation. 172

177 Importing and repairing shapes 173

178 In this workshop, you will learn how to: Import templates of different formats Check the validity of shapes Eliminate parasite elements Repair shapes Sew surfaces Cap holes Simplify parts Introduction This chapter deals with the methods available for importing and repairing external geometric data representing solid or surface shapes (this does not include the import of drawings). The aim is to take a file from a source other than TopSolid, extract the geometry and repair it in order to produce solid or surface-type shapes that can than be worked on as normal within TopSolid. This method should be applied when the normal import method does not function correctly, and simply using the File, Open function with the appropriate format does not provide satisfactory results. It should be also noted that even if the original system also uses the Parasolid accurate volume modeller format, we strongly recommend that you use a native Parasolid file format (X_T or X_B) as an intermediary, as this usually ensures immediate success. Communication difficulties The question might be asked why the problem of exchanging data between CAD systems has not yet been fully resolved, despite the existence of standard formats (IGES, STEP), and the fact that it is even sometimes possible to read the native format of certain systems (AutoCAD, CATIA, etc.) directly. It is important to dwell a while on this subject, as understanding of the difficulties involved will be of great help when one is confronted with problems in the future. A neutral file format definition standard is actually concerned with the syntax used (the way in which the geometry is described), and does not make any assumptions in regard of the quality of the information that is transported: The contents of the book is of little importance the important fact is that it does not contain any spelling mistakes! This is not due to an oversight on the part of those who designed the standard, but nevertheless proves to be the necessary condition to allow communication between several CAD systems with different characteristics. Thus, when TopSolid reads an IGES file, it not only has to interpret the file syntax, but also has to adapt the characteristics of the imported geometry to comply with its own demands. TopSolid is a modern application, it works with numeric values that are accurate to 15 significant figures, and manipulates geometry with a great deal of accuracy (0.01 µm); this is not necessarily the case with older existing design systems. Furthermore, TopSolid is permanently testing the quality of the geometry to ensure that it corresponds to the physical world and in particular that there are no auto-intersections (surfaces of curves that create a loop.). It is possible that a system that does not perform these checks may consider a geometry to be valid, whilst TopSolid considers this same geometry to be invalid. This may seem like a useless constraint that is imposed by TopSolid. However, is it better to live in ignorance and only discover at the end of the month that your bank account is overdrawn, or to be warned in a timely fashion as soon as a purchase might cause a problem? 174

179 Advanced Geometric Cleaning Module Manual repair of invalid geometric data can prove to be an extremely tiresome and time-consuming task, especially when there are a large number of elements to handle. In addition, by default, TopSolid is capable of performing a certain amount of repairs automatically. A specific module, dedicated to repairing geometries automatically, is also available as an option. This is the Advanced Geometric Cleaning Module (known hereafter as the AGC module). You can check to see whether it is active by choosing Tools, Options, Shape. This module implements complex algorithms that enable it to handle even more types of invalid geometry automatically. If you are required to import external data frequently, we strongly recommend this module. Some of the functionality described below is only available with the AGC module. This will be explained in more detail where appropriate. Non-associative mode Of the work modes available under TopSolid, the Non-associative mode is most suited to data repairs. It is actually useless to save the history of all the operations necessary to repair a model. In fact this may even damage the model. Also, it is advisable to change the work mode using File, Properties, General just after import, as soon as the TopSolid document has been created. When the model has been repaired, you will be able to switch back to whatever mode you prefer, and start modelling (associatively or otherwise) around a valid basic shape. Importing models Options configuration for interfaces can be adjusted: with File, Open and select Configurate button (active when IGESfile or other format is selected) or with Tools, Options, Interfaces IGES files Parameter restrictions Firstly, it should be clear that the IGES format enables two methods of representation of trimmed surfaces: parametric mode and spatial mode. Without going into detail, it is sufficient to remember that the mode that provides the greatest chance of avoiding problems is the parametric trimming mode, and this is selected by default. In addition, do not change the mode unless you are totally sure that the original system does not produce good quality parametric trimming and believe that you would probably be faced with a heavier repairs workload. 175

180 Smoothing polygonal trimming The parametric trims of a surface are represented by planar curves, which may have angular points (discontinuity of tangent), called vertices. Each segment between two vertices will correspond to an edge on the final shape, which it is possible to view using Curve, Other curves, Edge. Some CAD systems use polygonal parametric trims with a large number of segments, which therefore produce shapes with a very high number of edges. This produces models that are very hard to manipulate (handling time) and store (file size), and even worse, very difficult to sew (see below). For this reason, TopSolid enables these polygons to be smoothed; you simply have to select the Smooth trimming contours operation from the Other tab. If you do not know whether or not the originating system uses polygonal trimming, you need to perform a test on a test file: the number of edges on the shapes that have been extracted should be lower when the smoothing is activated. Postponing simplification It is possible to simplify the geometry automatically on import: This causes almost planar polynomial surfaces to be transformed into perfect planes. However, this presents the inconvenience of not knowing where a problem arises if a shape is invalid: was the shape invalid to start with, or has it become invalid as a result of the simplification? Furthermore, in the case of importing complex data, it is advisable that the Simplify geometry option is not selected on the Other tab, but that the simplification is postponed to a later stage (see below). Standard cleaning A certain amount of cleaning of the geometry can be performed automatically on import. Without going into detail, it is worth mentioning some tasks that are performed by the standard automatic cleaning routines: Division of surfaces containing discontinuities of tangency. Removal of self-intersecting areas that are outside the useful trimmed part. In contrast to what has been said previously about simplification, it is better to perform the cleaning operation immediately on import, and therefore to select the Clean geometry option on the Other tab. Moreover, some cleaning operations cannot be performed in a second session. Advanced cleaning If you have the AGC module installed, the cleaning operation will be much more complete (it will also take much longer). Without going into detail, the following comprise some of the tasks performed by the advanced automatic cleaning routines: Advanced repairs to parametric trimming Smoothing of surfaces that contain discontinuities of tangency Repairs to certain self-intersecting areas of surfaces. 176

181 Layers 998 and 999 When a surface trim is in such a state that it cannot be retrieved, TopSolid creates the surface without any trimming on layer 999. In (rare) cases where the support surface is an offset surface, the nontrimmed surface is created on layer 998. These surfaces must be trimmed using edges from neighbouring surfaces before being used. Do this using the Shape, Trim command with the option BY IMPRINTING CURVES. CATIA file For the reasons mentioned above, it is recommended that you do not select the Simplify faces option, but do select Clean faces. The CATIA interface also offers the option of sewing solid shapes automatically, which is of great help when it works! Nevertheless, experience shows that, except in simple cases, it is rare that a valid solid will be obtained from the automatic method without also performing the steps described below. Other formats As far as other formats are concerned, there are no specific characteristics to be aware of during import. Nevertheless, as cleaning will not yet have been performed, it is better to use the Shape, Manage, Clean geometry function in order to initiate subsequent cleaning. Verify shapes Visual verification Once the import has been completed, it is necessary to evaluate the state of the parts. The most important tools that you can use are your own eyes! If there are any misplaced or incorrect elements, these should either be deleted or, if possible, repaired. Verifying geometry The function Shape, Manage, Check geometry enables you to perform exhaustive geometric verifications (which may take a long time to complete: you can interrupt the function by pressing the Escape key). This function should be launched by clicking on the ALL SHAPES button with the Show problems option set to YES, and specifying the number of the layer on which invalid elements should be placed. If there is no invalid shape (the message No invalid shapes appears in the alphanumeric field), you can progress straight to the sew stage. In all other cases, it is recommended that you carry on reading this section. In order to identify the problems, you can print the LIST OF VERIFICATION RESULTS in the tree structure. Each geometrically invalid shape is referenced in the list, followed by a list of problems that were encountered (one line per problem). For each problem, a group is created with a short description of the problem, containing components that allow the default position to be located. 177

182 Eliminate Small surfaces Included amongst the elements that are considered to be invalid are sometimes tiny surfaces, or very fine bands. In addition, even if these are considered to be valid, the surface shapes with dimensions that are smaller than the level of precision that you wish to attain will not contribute to the parts and may make the sewing operation more difficult (see below). The easiest method is simply to eliminate these elements. In order to do this, the selection filter should be used with the Physical properties criteria and the SURFACE AREA option, and all the surface shapes with a very small surface area should be placed on a separate layer. Following brief visual examination, most of these surfaces can be deleted. Redundant surfaces It may also be the case that some surfaces will be duplicated, or that trimmed and non-trimmed surfaces may be superimposed (the latter overlapping the former): in such a case, the non-useful elements should be deleted, to avoid possible problems during the sewing operation. Non-useful surfaces In the same respect, some systems create surfaces representing the bottom of tapped hole threads during export: these surfaces should be deleted, or placed on an inactive layer for subsequent use; they do not belong to the actual part, and can cause problems during the sewing operation. Detection of non-useful surfaces can sometimes prove difficult in the case of a shape that contains many faces. It is also often the case that these surfaces are not detected until later, when the sewing operation fails: if this happens, you should consider whether or not there are still surfaces to be deleted, and return to this stage (or unsew the suspect area, then delete the non-useful surfaces, and re-sew everything). Repairs Need for repairs Although not obligatory, it is advisable to repair invalid shapes, when possible, in order to arrive at a zero error model (this ideal cannot, unfortunately, always be achieved). It is, therefore, worth while differentiating between several degrees of invalidity. A geometry may be so invalid that TopSolid is unable even to retrieve it (although this is rare), there are no other options but to reconstruct it, or to request a better version from the originating system (which can sometimes be awkward). A geometry may be retrieved, but declared invalid during the verification stage. It is still possible to work with the geometry, but it is probable that some TopSolid functions will not work correctly on this geometry (facetting, union, fillets, sewing, etc.), and it is, therefore, better to attempt to make repairs. The following sections provide some indication of how to repair certain types of error. Self-intersecting geometry When the fault is a self-intersecting geometry, this indicates that the surface is looping, and there is no simple method of repairing this type of problem. There are two alternatives open to you: Rebuild the surface, using the invalid surfaces as a model. Leave the surface as it is, hoping that the problem will not have consequences on the subsequent 178

183 actions to be taken. The more pragmatic attitude is to leave the element as it is, and to rebuild the shape afterwards, only if a situation occurs where progression is impeded (a Boolean operation fails, etc.). Parametric trim Most of the time, the problem does not arise from the base surface, but from the trims (e.g.: errors of the type The surface trims are self-intersecting), in which case it is sufficient to modify these. The easiest method is to use the function Shape, Manage, Trim UV, which enables the parametric trims to be edited directly. Spatial trimming When it is not possible to repair parametric trims locally, the simplest method comprises deleting all trims (using the function Shape, Other operations, Remove with mode remove = TRIMMING), and trimming the surface shapes using the neighbouring shapes (using the function Shape, Trim). It is also possible to use Shape, Manage, Repair sheet, this requires to have previously sewn valid surfaces, in order to use boundaries edges to define new spatial trimming of invalid shapes. Sewing Principle When all preceding stages have been completed successfully, the result is a fairly large quantity of valid, independent surface shapes. These, once sewn together, will delimit one or more solids (the final result to be obtained may also be a partially open surface shape, but in the main we will discuss the case of the solid, as the type of problems encountered are similar). The sewing operation consists of locating the topological connections that were lost during the transfer stage; this is done by joining edges that are identical to a given tolerance (specified by you). The aim, therefore, is to collect the boundary edges of surface shapes to be sewn together in pairs: the majority of problems that will be encountered will arise because TopSolid cannot find a pair of surfaces to join! We can differentiate two cases: When an edge is found on its own, it will not be joined, and will, therefore, form a part of the boundary edges of the final shape thus making a hole When more than two edges are found to match the given tolerance, joining them would produce a non-eulerian topology, which does not delimit a valid solid: the sew operation will fail. It should be remembered that the sewing operation is purely logical, and does not modify the geometry in any way (except when performed with the AGC module, see below). In addition if your trimmed surfaces are badly connected, even if you do manage to sew these together, the cracks that separate them continue to exist, a fact that can be verified by unsewing the shape. TopSolid is able to work with these shapes which have closed topologies, even through the geometry is not completely closed (the likelihood of success of Boolean and local operations will, however, decrease if the geometric connectivity is of very bad quality), but if you export these shapes to other systems (e.g. using IGES), the initial geometry will be restored, and the interstices will reappear. Method The most common method comprises sewing all the surfaces using the Shape, Other operations, Sew function (click on the button ALL SURFACES), progressively increasing the tolerance. Usually, we start off at 0.01 mm, and double the value at the start of each iteration, selecting the result from the preceding operation, or more simply, clicking on the ALL SURFACES button again. In the case of assembly of parts in contact, it is often preferable to consolidate all restricted surfaces belonging to a same part on the same level, and to hence produce sewing isolated on this level. This enables preventing invalid associations of surfaces during sewing (association of surfaces belonging to different parts). 179

184 It should be noted at this point that the sewing operation is capable of working on a single partially sewn surface, and therefore allows boundary edges that delimit holes to be sewn once the tolerance becomes large enough for these to be considered as coincident to each other. With each iteration, the number of solids created is displayed in the alphanumeric field, and when a solid could not be created, you will be given the number of surfaces with the number of internal holes. One small pitfall should be avoided: When we want to obtain a solid, and there is 1 surface with n holes, we actually have to cap n+1 holes, as one of the holes is counted as being the natural limit of the surface. Problem edges When TopSolid encounters matching edges (at a given tolerance) that it cannot join (as the resulting topology would be invalid), it does not join them and leaves them free, whilst indicating the problem with the message Problems have been encountered at some edges. In addition, conflicting edges are indicated by the creation of thick magenta curves that are superimposed. As was mentioned before, several causes may lead to this type of problem, and the only remedy is to clean the affected areas manually: Elimination of duplicate surfaces Elimination of non-useful surfaces Limitation of a badly trimmed surface In some cases, unsewing certain surfaces with edges belonging to these edges representing problems, then resewing them to the largest composite surface they have just been unsewn from, resolves certain topological problems (face-face error, inconsistent loops). Advanced sewing If you have the AGC module, the sewing operation also includes an automatic capping procedure. This phase consists of trying to automatically cap certain types of hole with an opening that is smaller than the sew tolerance, by modifying the trims of the neighbouring faces, or even by creating new surfaces. This avoids, at least partially, the laborious tasks described in the following paragraph. Capping models Usually, there will be a certain number of holes that cannot be filled automatically, simply by increasing the sew tolerance. The job must, therefore, be completed by hand, by creating new hole fill surfaces which must be sewn to the shape being repaired. These holes can be identified using the function Curve, Other curves, Edge and clicking on the EDGE CURVE button (in order to repair micro-holes, it is better to switch to the Create middle points = YES mode, and use a highly visible type of mark, such as a star.). Moreover, this function is suggested automatically at the end of the sewing operation: simply click on the COPY BOUNDARY EDGES WITH CENTRAL POINTS button. Once the hole has been identified, you can try to fill the hole with Shape, Other operations, Fill hole and if still unsuccessful, use the boundary edges to construct a valid surface, often using the Flat, Ruled or 4 curves shapes. The problem often arises from the fact that the surface that is produced is naturally self-intersecting, so the correct edges must be selected as a basis. Sometimes, the situation is so complex that the only way of escaping is to locally unsew the neighbouring faces using the Shape, Other operations, Unsew function and to place these on a new layer where they are easier to work with. Once the hole has been capped, the unsewn faces are re-sewn to each other, and then the whole element is re-sewn to the main shape. 180

185 Simplification When all of the preceding stages have been completed successfully, a valid shape is produced. This shape can be simplified using the function Shape, Manage, Simplify geometry. This function replaces polynomial planar surfaces with analytical planes (less demanding of memory and allowing faster handling) and recalculates certain edges by intersection between neighbouring faces. In addition, the neighbouring faces that share a base surface are joined into one single face. If you have the AGC module, the handling is faster, and in particular the polynomial surfaces that represent an analytical surface such as a plane, cylinder, cone or sphere with a given tolerance are replaced by an analytical surface. Simplification is a complex operation, which can sometimes raise cases of invalid geometry, so it is recommended that a verification is performed again to ensure that this is not the case. If invalid elements are found, the simplest solution is not to perform the simplification (and it is useful to have saved the document just before starting the simplification!), but it is sometimes a pity to undo the simplification because of one unfortunate micro-surface that does not fit The solution, therefore, consists in performing the simplification before the sewing operation, avoiding applying it to the areas that fail. This can nevertheless prove to be laborious, as it is necessary to batch the simplification and verification and to undo if the verification detects something invalid. 181

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187 Importing IGES Topics covered: How to import an IGES file: to import an IGES file we need to use the function File, Open. How to create a solid from surfaces: in order to transform surfaces into a solid, we need to sew them and fill in any holes. The file Clamp.igs is a transfer file containing a network of surfaces. We are going to use these surfaces to realise a solid. How to import an IGES file 1 Import the template Use the function File, Open. Select the file type IGES, and open the file Clamp.igs. 2 Enable all data Once the file is open, use the layers editor to check which layers are used. In the file Clamp.igs, layer 15 should be activated as it contains all of the surfaces. How to create a solid from surfaces Sewing 3 Initial sewing Choose the function Shape, Other operations, Sew. Use this function in NON-ASSOCIATIVE mode in order that the base surfaces that do not possess any construction history are not linked once the sewing has been completed. Then in the dialog row, leave all settings at default and sew ALL SURFACES. After calculations are completed, the sewing report is: Tolerance = 0.01mm solids count = 0 surfaces count = 1 holes count = 4 Identify holes After the sew operation, TopSolid indicates that the part has four holes. These must be identified and capped. 183

188 4 Identify holes In order to do this, increase the thickness of the current line type, then click on the COPY BOUNDARY EDGES button, which appears at the end of the sewing operation then click on STOP. It is also possible to use the Curve, Other curves, Copy edge function clicking on the BOUNDARY EDGES button and designating the appropriate part. Cap holes with surfaces There are several techniques for capping holes: Duplicate an existing area by symmetry Create a swept surface Create a ruled surface Create a 4 curves surface Duplicate an existing surface by symmetry Hole number 1 can be capped by copying the triangular symmetric surface. 5 Copy the missing symmetric face Use the Shape, Other shapes, Copy face with the TRIMMED face option to duplicate the surface. 6 Duplicate by symmetry Then use the Shape, Other operations, Transform function. Click on the previously duplicated surface, choose the MIRROR SYMMETRY transformation and select the plane XZ. 184

189 Create a swept surface Hole number 2 can be capped by a swept surface, a guide curve (A) and two section curves (B and C). 7 Create the swept surface Use the function Shape, Other shapes, Swept and. Click on guide curve A using the sweep mode NORMAL, then AUTOMATIC. Create a ruled surface 8 Construct the ruled shape Use Shape, Other shapes, Ruled to cap hole number 3. Select the two smaller curves and start the calculation, leaving the parameters at default. Create a 4 curves surface 9 Fill with 4 curves Use Shape, Other shapes, 3-4 curves to cap hole number 4. Select the 4 joining curves in any order, and click on OK, leaving the synchronisation options set to default. Sew Important note: You can also use Shape, Other operations, Fill hole and adjust tolerance. Now that the holes have been capped, we need to repeat the sewing action to produce a solid. 10 Final sew Use Sew in NON ASSOCIATIVE mode. Leave all settings at default with a tolerance of 0.03 and sew ALL SURFACES. After calculations are completed, the sewing report is: Tolerance = 0.03mm solids count = 1 surfaces count = 0 Add operations and analyse As the part is now solid, it is possible to create operations, such as drillings, fillets, drafts, etc. 11 Adding operations Add a fillet of 2mm on the linear edge. Drill a hole of 2mm through the rectangular face at 2mm and 16mm from the boundary edges. It is also possible to analyse the properties of this part. 185

190 12 Analyse the mass of the model With a steel construction, the mass is g. 186

191 Importing DWG Geometry Concept to introduce: How to retrieve a 2D file originating in another CAD system. How to configure contours. Modelling the part. The Wheel.dwg file is a file that has been created entirely in 2D; we will retrieve the different views, and rebuild the wheel as a parameterized 3D volume. 1 Importing the dwg file Start the File, Open function. Open the File type list and select AutoCAD - DXF / DWG (*.dxf, *.dwg). We are about to rebuild a volume model, so we must confirm the default options: Unit = Auto Standard= Auto Then click OK to validate. After retrieving the data, the following drawing is obtained: The result of the import can be displayed by clicking on YES to the following prompt: Display the contents of the results file This information can be of use in the case of error messages that arise when importing the DWG file. The import result file is a text file in ASCII format, and has the same name as the DWG file that was imported, with the extension.res (in our case Wheel.res); the file is loaded in Windows Notepad. 187

192 Parameterization of contours We will now delete any geometry that is not of use for modelling the solid shape. 2 Sorting elements Choose Delete and only keep the following elements (contours for each view). 3 Creation of coordinate systems For each of the views, create a coordinate system using the Tools, Coordinate system menu item, then choose an intersection point. 4 Parameterization of the first contour Trim the horizontal line in respect of the 2 vertical lines using Curve, Trim in order to obtain joined elements. Start sewing the curves using Curve, Other operations, Sew in NON- ASSOCIATIVE mode and check the option Delete original curves. When the sew operation is complete, select the REBUILD option; this option corresponds to choosing the Curve, Other curves, Rebuild function. The results of the sew operation are displayed in the message field at the bottom of the screen. The contour created in this way is an associative contour; it can be constrained using driving dimensions. Please remember that contours must be sewn in their respective coordinate systems. 188

193 5 Parameterization of the second contour Now Sew the second curve using the same options, and add its controlling dimensions (modify the 4mm dimension by adding a symmetry constraint in respect of the Y axis). These contours must be sewn in their respective coordinate systems. Modelling the wheel We will now delete any geometry that is not of use for modelling the solid shape. 6Revolved shape For the first contour, Revolve the curve around the X axis of the coordinate system using. For the second contour, you must start by orienting it by rotating the coordinate system of the view by 90 around the Y axis. 7 Orient the coordinate system Use the Modify element function, then click on the coordinate system to cause the following window to appear: Click on the Y button to revolve the coordinate system by 90, the coordinate system is modified instantly. After confirming using the OK button, all elements linked to the coordinate system will also be revolved through

194 8 Trim Now apply a trim using Shape, Trim with the TRIM WITH A SWEPT CURVE option and Sweep mode = EXTRUSION, on the shape rotated by the second contour (it may be necessary to invert the extrusion direction). The parametric part obtained in this way can be modified as required, used in the assembly, transformed into a standard component, etc. 190

195 Tool box for shapes Topics covered: Tool box functions to work with surfaces 1 Open the part Select the ToolBox.top file with File, Open. Open the construction tree (CTRL+²). Then Select the part on the screen. Analysis: It is a basic part. The part may be the result of an importation by TopSolid interfaces (IGES, STEP ). 2 Modifications Expand the tool box menu Shape, Tool box by clicking on. Position the menu on your screen. Redimension the face, then Select cylindrical face 1. Enter OK then the new diameter 10mm. CRITERIA constraint on the diameter: enter equals then 8 and then OK. Select the part (the 3 other open pocket diameters must become red) then the new diameter 10mm and OK. Remove faces then select the 3 faces of chamfer 2. Healing=Fillet then OK Reblend radius then Select fillet 3 and OK. New Radius = 12mm then OK. 1 Constrain face, then select cylindrical face 1. Type of constraint = Alignment, select cylindrical face 3. Constrain face, select face 4. Type of constraint = distance, select the bottom of the part as the reference face, then new distance = 5mm. Reblend radius then select inner fillet 5. New radius = 7mm Reblend radius then select outer fillet 5. New radius = 12mm

196 3 Other holes Switch to top view. Use Stretch, click 2 points to obtain the rectangle selected. X- then translation distance = 15mm. Select the part. Move Feature or Face, select loop 1 then the bottom face of the part as the trim face, and then OK. TRANSLATION, Y+ and 15mm. Move Feature or Face. Move = face, then select cylindrical face 2. Translation, Y+, 10mm. 1 2 The final result must be as shown here: Save the file under the name ToolBoxINDB.top. 192

197 4 Open ToolBoxTraining.top file. Activate levels 2 and 3. Edit in the tree: The PINK part to see that it is basic Then the CYAN part, a part constructed in place, based on the PINK part (contour and drill hole concentric to the spot faced hole) and depending to the tools of the 4 screws). Window, Tile vertically Activate the assembly Use Shape, Manage, Replace geometry. Shape to be replaced: Select the PINK part of the assembly. Replacement shape: Select the INDB shape. Option: NO TRANSFORMATION Then OK. In the INDB document, select the edges corresponding to the highlighted edges in the assembly. Result: You must obtain the result shown here. Only the edges required for the construction in place are requested, i.e. the 4 upper circular edges of the holes as well as the lower circular edge of the spot faced hole. In the aim of testing another possible use to Cancel the operation. Restart the previous procedure, this time selecting the following option: plug all in the dialog box (If the edges or faces no longer exist (function deletion) select the no replacing edges option or define the equivalent). Result: The procedure is longer. TopSolid first asks you for the face equivalent and then the edge equivalent. Only to be used if you have created an external associativity (layout, assembly by component) For machining, instead use the you to reconnect the machining operations. part/ compare and replace function which will allow 193

198 In the aim of testing another possible use to Cancel the operation. Open ToolBoxTraining.dft. Restart the previous procedure, this time selecting the following option: Plug those being locally referenced in the dialog box. Result: The procedure is at the halfway point compared to the two previous ones. Indeed, TopSolid also asks you for the edges required for the associativity of the 2D dimensions. In the aim of working with a problematic case, use to Cancel the operation. Close the layout document ToolBoxTraining.dft Restart the previous procedure, this time selecting the following option: Plug those being locally referenced in the dialog box. Open ToolBoxTraining.dft. Result: Several dimensions are to become orange. This means they are disconnected. To reconnect them, use Edit, Modify element on the disconnected witness line and then on the new edge. The dimension must then return to its normal color. File, Close all, tick the Apply to all documents option. Then NO. Open ToolBoxTraining.dft. File, Reroute then select ToolBoxTraining.top in the drop-down list. BROWSE. Then select ToolBoxINDB.top Result: All the dimensions are reconnected correctly. Indeed, all the modifications to the new 3D file have been made in TopSolid using the tool box, in this case When the new document is from a different software program, opt for the replace/ geometry function (opening the previously referenced documents, if any). When the new document is from TopSolid, opt for the reroute function (as the identification of the entities does not vary). File, Close all, tick the Apply to all documents option. Then NO. 194

199 5 Trimming Open ToolBox- Training.top file. Create a curve similar but not necessarily identical to the one here. Then extrude it. 1 2 Shape, Tool box, Replace face Face to replace: face 1 Replacement surface: face 2 Shape, Manage, Isolate part. Select the lower blue plate. Create surface 3 Replace face 1 by face Result: Only the upper part is affected by the Replace face modification. Indeed, as from the Isolate part function, the lower part is completely autonomous (yet still parametric). NOT TO BE CONFUSED WITH THE BASIFY FUNCTION. 195

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201 Advanced 2D Import Topics covered: Rebuilding of 2D elements. Repairing and creating 3D from 2D. 1 Import 2D DWG File, Open Select the Geometry.dwg file. Click on CONFIGURATION. Set the options as shown above then OK. Re-enter OK. Keep the default settings (Unit:auto; Standard:auto and Create views: NO) then OK Result: The.dft and the.top are not connected. The 2D elements of the design document are merely copied into the draft. The dimensions are converted and may be modified. File, Close All and NO. Restart the operation, this time using the following options: Break dimensions: YES Break groups: YES (in the dialog box) create views: YES Result: The.dft and the.top are connected. We have opted to load the AutoCAD paper space (the object space is necessarily loaded). TopSolid will therefore create 2 files (a.top corresponding to the object space and a.dft corresponding to the paper space). Recommendation: In the Open window, you may select the type of file to be generated during an importation. Here, TopSolid'Draft (Set on TopSolid'Design by default) 2 Advanced 2D Open Advanced2D.top file. 3 Modifications on basic curves (level 1) Analysis, Geometry on the various elements OR - Edit the various elements (in the tree) OR - F2 then pass to an element OR - Analysis, Element on the various elements 197

202 Result: All the elements are basic, even if they are recognized as simple curves (line, arc, circle, and ellipse). The dimensions obtained are therefore driven (yellow). Using the Edit, Modify element modify the following elements: A The radius option on the arc. On the arc, extract and healing = YES Displacement of ends B Change the values on the chamfer The extract option on the chamfer C On the circle (value, angle, passing point) D On the arc (value, angle) E On the ellipse (angle, radius X, radius Y) F On the curve (option ) function, B Curves, Manage, Rebuild. On elements A to E. Arc and lines option for curve F. Tools, Dimension on the curve. Result: The elements are now parametric (green driving dimensions). The advantage is that the Modify Element function may be used to do almost everything. Difference trim extend cut A B C D E F G H 4 Trim Using the Curve, Trim function, modify the following elements: A On the horizontal line 198

203 B C D E F On the horizontal line, automatic option On the horizontal line, share option On the arc The circle by 2 points The circle by the curve The 3 H lines by the V line 5 Extend Using the Curve, Extend function, modify the curve: G Left part tangent, Right part curvature 6 Cut Using the Curve, Cut function, modify the curve: H ALL CURVES option, ONE CURVE option Result: The Trim function is for general use; Extend and Cut are for use in 2 specific cases. 7 Difference between 2D pattern, 3D pattern and propagate operation A B C D E F 8 2D Pattern Using the Curve, Pattern function, create: A B C A circular pattern (nb=4) A linear pattern (nb=4; step=20) A double mirroring pattern 199

204 9 3D Pattern Using the Curve/ Other operations/ Pattern function, create: D F A mirroring pattern A circular pattern then subtract 10 Extend Having first executed a trim by sweeping curve, E Execute Shape, Propagate operation (circular) Result: There are various ways to obtain the same result. By preference, use the 3D functions which may be directly modified and simplified in the construction log. 11 Sewing Open Layout.dwg. A B Examine zones A and B. Result: Zone A contains non contiguous curves that must have been created without being hooked to objects. Zone B contains broken and non contiguous curves. Curve, Other operations, Sew. NON ASSOCIATIVE option. Select the curves. Tolerance=2. 200

205 12 Closure of zone 1 curve Curves, Other curves, Around a point. Select the curves required for the closure of zone 1. Click a point inside zone Closure of zone 2 curve Curve, Manage, Rebuild the zone 2 curve. Edit, Insert to close the curve. 14 Free Closure Close the other curves, if necessary 15 Raising walls 3 Shape, Extrude Height=2500. the walls. Recommendation: Obtain height of subsequent walls by clicking on the previous walls. 16 Modifying walls Modify, Parameter. Click on one of the walls. Enter Attribute, Visibility. Elements to make invisible option ELEMENTS TO MAKE VISIBLE SHOW ONLY INVISIBLE ELEMENTS option. Click the contour corresponding to the zone 3 wall. Quit option. Of course, in this case, there was a simpler method; the function (control element) would have been quicker. The previous method is only to be used when all the driving elements are in the invisible space. Avoid using Vis=Hid as sooner or later it is bound to cause complications. Switch to top view. 201

206 Edit, Stretch parents. Click 2 points defining zone 3. Option X+. Distance Make a window surrounding all the elements. 17 2D to 3D migration Open base.dwg. 18 Method 1: by parameter on auxiliary view 3 Break the 3 views. Curve, Manage, Rebuild. NON ASSOCIATIVE option. OK. ALL CURVES option. Tolerance=0. 4 Shape, Extrude Select curve 3. 1 Parameter then Distance 2 between point 1 and 2. Name:h Stretch parents. Click 2 points defining zone 4. Y+ option. Translation distance=20. Elements to transform window surrounding the top view. Result: This method is better suited to 2 ½ D parts for which the main view contains the main part dimensions. 202

207 19 Method 2: by reconstruction and then modification of the coordinate system Tools, Coordinate system, create coordinate systems at points 1, 2, 3. For each view: 1 2 Coordinate system, Current the view coordinate system. Shape, Other operations, Sew in NON ASSOCIATIVE. 3 Shape, Manage, Rebuild (if necessary) the elements not reconstructed by sewing. Then rotation of coordinate systems: Modify, Element. Coordinate system 2-90 on Y Coordinate system 3-90 on X Shape, Extrude the contour of the face view. Height: click on the high point of the top view. Shape, Trim. By sweeping curve option to create the auxiliary view drill holes. Result: Goes a little further than the previous method. Allows the possibility of realigning views using Move parents on the coordinate systems, not dynamically. For complex parts, use Shape, Other operations, Intersect. 203

208 20 Method 3: using the curve/transform option: positioning Curve, Transform. Positioning option. Click point 1 then point 2 and finally point 3. Point 1 then &0,0,10 and finally point 2. Select the left view elements. Repeat the same on the top view Result: Universal method (allowing any 3D spatial transformation to be executed). Very useful in simple or double balancing with any angles General summary: Whatever method is used, always reproject the 3D part and verify that it is OK (dimension forced, view not aligned). 204

209 2D Drafting 205

210 Concept to introduce: Opening a new TopSolid Draft document Creating a 2D view Creating an auxiliary view Modifying the scale of the document drawing Creating geometry Anchoring automatically on views Creating perpendicular views Inserting fastener element Create a detail view Move views This exercise provides an example for production of a pure 2D drawing. The exercise introduces the idea of a parameter as a means of maintaining correspondence between the views. Use of parameters is not always needed or called for, and modifications are then managed as on a drawing board. 1 Open a new TopSolid Draft document Open a new document on the Draft tab. Select one of the standard templates Associative horizontal A3 mm. 2D view The 2D view function enables you to define a drawing space to characterize a view. All the lines in this view can be moved simultaneously. You can change the scale in respect of the document scale, using the Modify element function by clicking on the format box, or change the proportions in respect of the other views. 2 Create a 2D view In this exercise, use the 2D view function to create a main view and position it in the document space, for example at the top left of the document. This will be the face view. Auxiliary view The auxiliary view function enables you to define a view maintaining the alignment in respect of another view. 206

211 3 Create an auxiliary view In this exercise, create an auxiliary view to the right of the 2D view (left-hand view), create another below (bottom view) and another to the bottom right (to provide a perspective view). Modify the scale of the document drawing The scale of your draft document is that which is specified in the drafting border; it controls the size of all 2D views. 4 Modify the scale To modify the scale, the format and properties of the document box, use the Modify element function, and click on the document box. Modify scale to 1. 5 Create geometry In the front view, use the Contour function and build a contour using the option RECTANGULAR. Construct the rectangle, aligning the bottom along the origin. Use the option AUTO DIMENSION to constrain the rectangle. Build a second RECTANGULAR Contour with one point common to the first rectangle. Build a third Contour element using the right-angle shape. Select the existing contour points using the left mouse button (use the middle mouse button for an independent contour). 6 Copy geometry Use the Edit, Copy command to copy the first rectangle with the SYMMETRY option in respect of the Y axis. Use the Edit, Duplicate function to copy the other two contours. Dimension the length of the copy of the first rectangle. 207

212 7 Modification and dimension Dimension the length of the copy of the first rectangle from 55 to 70mm. Construct a chamfer on the origin right angle from 5mm to 30. Construct the missing segments using the Line function. Create hatching on the sections using the Hatching area function in the Detailing menu. Set the hatching pattern in the attribute bar. Dimension the central boring diameter to 20mm using a symmetry CONSTRAINT. Anchor automatically on views The Automatic 2D view selection function enables you to activate and deactivate the automatic anchor for lines on the nearest view by activating its point. Create top view 8 Automatic selection De-activate the Automatic 2D view selection mode. 9 Sketch line Set the coordinates for the top view as current using the Coordinate system current tool. Construct sketch lines by taking vertical alignments with front view. Construct a horizontal sketch line passing through the origin of the coordinate. Construct an offset for BOTH SIDES at 90mm. Then construct a Contour based on the sketch lines of the decal base. Construct circles centred on the origin, and tangents to the corresponding sketch lines. Define two chamfers using the chamfer function in the Curves menu. Create side view 10 Base lines Set the left view coordinates as current and draw a vertical sketch line. Draw two Parallels to this line using the BOTH SIDES option, click on the 120mm dimension on the top view to define the distance. 208

213 11 Contour on sketch line Construct a Contour on the sketch lines of the decal base. 12 Finishing the contour Use the Duplicate function in the Edit menu to copy the right angles and small rectangles with the TRANSLATION option from the origin of the right-hand coordinate towards the origin of the left-hand coordinate. Construct a Contour between the copies of the right angle. Construct the missing Lines and modify the type of line for the copies to dotted. Construct 2 Parallel lines at the edges of the decal to represent the chamfers. Use the Merge function from the Parameter menu. Keep the origin parameter by selecting the chamfer line and choosing LENGTH. Apply this value to the sides of the parallel lines. Reactivate the Automatic 2D view selection. Fasteners element 13 Insert 2D screw Use the include standard function from the Assembly menu to include fastener screws. Select AFNOR2D and, in the front view, include a curve view M5x20 screw and position it on the right angle line using the middle mouse button. Press STOP and select the Drill hole and Tap processes, and apply to the parts. Press STOP to position a second screw. In the top view, include the same screw in the top view to a point on the vertical of the centre of the bore. Repeat the screw in a Circular manner over 360 with 4 copies. 209

214 In the left view, include a screw and position it on the side of the view. Use the Ungroup function in the Edit menu to break up the lines, then the Group function of the same menu to join the lines to the head of the screw. Use Copy to move the screw to its position. Use Duplicate to copy the screw head with symmetry. Delete the original screw. Move the sketch lines and constraint dimensions into the invisible space using the Visibility function on the Attribute menu. Use the Selection by Type (Dimension and Lines) from the tools in the toolbar on the left. Designate supplementary lines to hidden or inverse. Draw axis lines using the Axes function in the Curve menu. Create a detail view A detail view is an enlargement of a section of a view. The software enables you to cut a section of the detail using a circle, rectangle or a pre-defined curve. 14 Detail view Choose View, Detail view and the CIRCLE option and position the centre of the circle around the area to be enlarged. Then position the detail view. Move views The Move parents function is used to move the position of a view during the drafting process. 2D views are independent, and when moved, carry with them the auxiliary views which are attached to them. 210

215 The Auxiliary views are dependent on their reference view and maintain their alignment in respect of the reference view. It is possible to cancel or re-establish alignment using the Modify alignment function from the view menu. It is possible to adjust the alignment for several views using the Adjust alignment function. 211

216 212

217 Title block 213

218 Topics covered: Create a title block Learn the related formatted texts. 1 Creating the title block Create a new document Draft and select Without template in the list. In the new window, the A4V paper size is preferable. A format appears. To personalize it, use the Modify element function. Tick options as appropriate in order to eliminate graduations around the border. In the Detailing menu, select the Title block function. Define the length and height of the title block, and also its hook point. In general, click on the HOOK ON BORDER button for the title block to stay aligned on bottom right of the border. Define the cells for the following cutting types: horizontal, vertical, regular Note: New cells may be created after leaving the function (using the Title block cell function). To modify the cell size, use Modify element and click on the horizontal and vertical cross-sections of the cells. To delete a cell, use the Extract element function. 2 Insert a text, a formatted text, a logo or a drawing To fill in the title block: use the Insert function and specify the title block Specify the cell into which the text or formatted text is to be inserted. Key in the text directly or select the formatted text in the list provided. 214

219 Once the formatted text has been selected, it may be adjusted using the window that appears Note: In the list of formatted texts, the PROPERTY line allows access to the information defined on a part in the 3D file (name, reference, material, etc.). This information automatically appears in the title block whenever a part or assembly is projected. More than one element may be inserted into the same cell. Draw the element outside the format. Group the elements concerned using the Group function located in the Edit menu. Insert the element into a title block cell (specify the appropriate title block and cell) Adjust its position using the dialog box. Hide the geometry located outside the format using the Visibility function in the Attribute menu. 215

220 The logo may also be a bitmap format file (bmp, tiff, jpeg, png ) and inserted in the same way as a cell. The formatted texts and the logo may be repositioned once they have been placed in the cells. Click on the text to be modified using the modify element function. 3 Save and rename the title block Save the file in the Missler\Config\Template directory. For different formats, simply modify the properties of the border and save the file with the desired format. Note: Remember to set the different options for the properties of the dimensions, texts, bills of material indexes via the File, Properties function. Name the title block as a new document and select the desired template in the list of user templates. 216

221 4 Using the title block To fill in the title block, select the Properties function in the File menu. Click in General information, and fill in the field. The information will appear in the title block. Note: only information such as author, company name, address 1 and address 2 are saved when using a format. The creation date uses the computer date as a reference. 217