There are 8 main topics in this training session which focus on the Sketch tools in IRONCAD. Content Sketch... 2 3D Scene Background Settings... 3 Creating a new empty Sketch... 4 Foam with cut out for Customer Product... 7 Control the Spin Wizard rotation axis... 18 IRONCAD Options, General... 20 IRONCAD Options, Interaction... 21 IRONCAD Options, Color... 22 Solidmakarna English Sketch Tutorial Videos: Also remember that we have an English multimedia based training material that you can find on the Nefab Intranet. From Section 13 (Day 1) we are going through the basics and some more advanced parts of how to work with the Sketch in IRONCAD. You can also use the free online training material found here: http://www.ironcad.com/training/icintrotraining.html#p=15 1
Sketch The Sketch is a grid plane with 2D Curves which is the main base in features like Extrude, Spin, Sweep and Loft shapes. It can also be used to create a none 3D model in IRONCAD, which is shown in the 3D scene as 2D curves on a (not visible) plane in space. Used as references for building layouts (walls, windows and pillars etc) or as the rotation workspace for a robot or as logos placed on a face of 3D models. Sketch or 2D Shape or Cross-Section? In versions before v2009 (v12) there was nothing named a Sketch in IRONCAD. The grid plane of an existing feature was called Cross-Section ( to edit the Cross-Section of this feature ), while creating a new part with a grid plane was called a 2D Shape (I place a new 2D Shape here). Those names are still valid and used. With the new interface using Ribbon bar tabs introduced in v2009 there was a tab called Sketch, which collects all tools working with a 2D Shape or a feature Cross-Section in one place. There are no other differences than the names, but it can be a bit confusing calling the same thing by two/three different names. In this document Sketch will be used as far as possible, since it can be considered an umbrella name for them all. Toolbar and Ribbon tab When entering the Sketch from a feature or when creating a new feature in IRONCAD you mainly use the tools available from the Icon Toolbar or Ribbon Bar tab. Most of the sketch tools are gathered under both the Sketch tab in certain groups and in different toolbars named 2D Technical Drawing (Drawing), 2D Editing (Modify), 2D Constraints (Constraints) and 2D Display (Display). The tools in the toolbar named 2D Construction are listed in the Ribbon bar Drawing group under the Center Line drop down button. 2
3D Scene Background Settings Due to the bright default colors of Sketch elements like curves and dimensions it might be good to set a darker background color before editing, to get a better contrast between the Sketch elements and the background. Right click in the background and choose Background Use a Color and set it to darker Top and Bottom colors like black and dark gray. It is also possible to alter the default colors of the Sketch elements under the IRONCAD Options, which is explained later in this document. Also remember that all these settings are pre-set by the the Nefab specific instructions running the CAXA Live Update installer. 3
Creating a new empty Sketch Use the Create 2D Sketch button to create a new empty standalone Sketch part. A standalone Sketch part has its own icon in the Scene Browser history tree and is named 2D Profile. Placement of the Sketch When creating a new Sketch there will be some placement options presented in the Property Browser. Usually you just have to click in the background or on a point or face of a model in the 3D scene, instead of choosing a certain Placement Type that is listed in the Property Browser. We also recommend you to select the option Finish command if conditions are satisfied, which will automatically go forward once you click in the 3D scene. If you don t choose this option, you will always have to manually finish the command on the top left green confirm button. Instead of choosing any of the placement options, using the Triball will almost always be faster. 4
Drawing Grid Too Large for View TRAINING SESSION It is also quite common that you are presented with a Drawing Grid Too Large for View window with some options, before the Sketch is created. The reason this comes up is that the complete square grid plane for the Sketch doesn t get room on the screen. Usually there s a reason why you have zoomed in to a certain position, why we recommend you to Continue without change and also Do not show this dialog again. The camera position will then not be changed by the program and it will remember this option for the future. The options can be changed in the IRONCAD Options (see below). The other options are Expand view to fit grid - which will zoom out the camera enough to see the whole Sketch grid plane and Shrink grid and grid resolution to fit view which will make the Sketch grid plane and grid resolution smaller instead of altering the camera view. None of these two are usually what you want IRONCAD to do. This can be controlled from the IRONCAD Options under the tab Interaction, where the option Prompt will show the message window again. As said we recommend the options Continue and Point from the Default Location Type drop down menu, which is the fastest way to get going. 5
Creating and modifying Curves in the Sketch TRAINING SESSION When entering edit mode, the tool icons in the Sketch toolbars are activated (when using the Toolbar UI). If you are using the Ribbon bar UI, the Sketch tab will automatically become selected by the program, if it was not already selected. Finish the Sketch To finish and confirm the changes in the Sketch, use the Finish button, which is reached from different locations (depending on UI). <- Using the Ribbon Bar UI there is a Finish button available at the top left corner. Cancel is located in the same menu. The same options can also be reached by right clicking in the Sketch background -> Using the Toolbar UI there are Finish/Cancel buttons in the Edit Cross-section windows available on the right side of the screen. 6
Foam with cut out for Customer Product A good start for a foam part is to drop a Block from the Shapes catalog on the customer product. Make the Block large enough to surround the customer product. Extrude Wizard The Extrude Wizard is a fast and easy way to create a new part or to add or remove material to/from an existing part. All settings can be applied from start or easily edited afterwards. To create an extrude shape that removes material, start the Extrude Wizard and click on a face of the part where you want to remove material. The Extrude Wizard will then start and guide you through a 4 step window with options. Choose Remove material. At this stage you can either proceed to Next step with options, or just Finish and start drawing the curves in the Sketch. All these settings can be altered afterwards. The Extrude settings has the Edit Feature Options where you can change between add or remove material and the depth. Use the Triball to change the position and direction, while the Sketch settings controls the grid display and size. 7
Project Curves TRAINING SESSION Use the Project Curves tool to steal the contour from the customer product into the Sketch. The Project tool can be found in different locations, but a fast way to find it (and many other tools) is by using the S menu or Popup Floaty as the menu is actually named, by pressing the [S] key on the keyboard. It us usually faster to click on a face than on individual edges one by one. The whole outline will then be projected with curves. Display Settings Remember that you can change the Display settings in the Property Browser if you want to hide geometry that you are not working with. In this case the Hide Edited Part is useful, since you are only interested in the other parts in the 3D scene. 8
Select Outline TRAINING SESSION Since the faces were selected with the Project tool you will get many curves that are not useful for this shape, which needs to be removed. A fast way to select many lines at once is by using the outline option. Either right click on one curve in the chain of curves and choose Select Outline, or double click on one of them. Another problem is that the whole chain of curves is selected, we only want to remove a part of the outline - the curves on the inside. A fast way to do that is to disconnect the curve that ends the outside chain on each side and then remove all the curves on the inside. As a result, the knee point between those curves is colored red to mark that it ends a curve (chain). 9
Select the outline of the inside curves and remove them. TRAINING SESSION Trim After some adjustments have been done it might be good to clean up all unwanted curves by using the Trim Curve command. A fast way to reach it is to use the [S] menu. Remember that you can press and hold the left mouse button and continuously delete curves by moving the mouse cursor on curves. You can of course click on curves one by one to remove them as well. 10
Polyline With the Polyline command you can draw extra curves where needed or when the Project command creates splines which are not possible to edit or trim. Make sure to use the help given by the SmartCursor function, which will guide you with green dashed lines when the curve you draw is parallel or perpendicular to the other existing curves in the Sketch. Hold down the [Shift] key to temporarily remove the SmartCursor function while creating any kind of curves. It is also possible to turn off the SmartCursor permanently in the Sketch Snap settings. 11
Offset When there is an unbroken chain of curves in the Sketch, all around the customer product, it might be good to set a 2 mm offset of the outline. Select all curves and then start the Offset command. Already in the preview (blue dashed lines) we can see that there might be some problems with the offset due to certain curves. This can be fixed before or after the offset, but usually it is faster to ignore problems like these and fix the resulting curves after our offset has been made. It might also be a difference between the preview and the final result, since the preview is not always as accurate as the final result. This is due to performance reasons, which is also the case with the feature tools preview. 12
In this case there are both missing lines and overlapping lines. The reason seems to be splines and possibly something that can be considered reported to the developers for improvement. It is almost always good to save the original contour curves, why the option Use Outline for Construction Only is useful in this case. Right click on any of the curves of the inside chain of curves to change to Construction curves. The result is blue colored Construction curves which will not create any 3D geometry upon finishing the Sketch. 13
Remove the overlapping curves and draw new curves with the Polyline tool. The Polyline tool also includes drawing arcs. Hold down the left mouse button and move the cursor away from the start point of the curve when the straight line has transformed into an arc, release the left mouse button. Then click and confirm the second point of the arc as usual with the left mouse button. There is also a button to toggle between lines and arcs in the Property Browser, when the Polyline tool is active. 14
Fillet TRAINING SESSION Using a Fillet radius in corners is usually better than arcs. A reason is that the Fillet can be considered a feature more than its own kind of curve, which does not affect how a straight curves behaves when it is being edited or dragged with by its Shape handle in 3D at a later point. Place the Fillet between two curves that extends against each other for a corner. The corner does not need to be closed, since you can click once on each curve to close them. You can also replace an existing arc in a corner, which will be automatically disconnected from the curves, when the two straight curves are selected. Then remove the arc. If a Fillet is removed the knee point will be restored. It is useful to apply the Lock radius setting, which will only need a single click to apply the Fillet on knee points, or click once on the two curves that will be joined, without having to insert the radius value again. 15
Curve Dimension TRAINING SESSION It is possible edit the length of multiple curves using the Curve Dimension tool. The tool can be activated and deactivated in different locations. Also when a curve is being created the Curve Dimension can be controlled in the Property Browser. Select multiple curves by holding down the [SHIFT] key. The last selected curve will show its Curve Dimensions, or if you have box selected a number of curves, deselect and re-select the curve you want to control. Also remember that the direction of the length change is controlled by the side of the middle of the curve that is selected. Double click on the dimension text to edit the dimension in the direction it was selected. All other selected curves will move with the change. 16
Shape Handles TRAINING SESSION When the outline is completed and the Sketch work has been finished, it is still possible to edit the curves outside the Sketch using the Shape handles. The Shape handles are also used as a way to control measures between geometries. Select the Extrude shape - sometimes it is easiest to find and select in the Scene Browser-> When the mouse cursor crosses a sketch curve a red Square Handle appears in the middle of the curve. By right clicking on the handle and choose Edit Distance from Point -> Point you can control/edit the distance between the curve and the customer product, if it needs to be altered in certain places. If the Shape handle does not work and no change is made when it is modified the reason is probably that there are no Fillet radius s set between the curves attached to the curve that is being changed. If there are arcs or splines the Shape handle will not be able to move them, instead it will be trying to modify them. In that case you either have to make the change in the Sketch, or replace the arc/spline with a new Fillet radius instead. 17
Control the Spin Wizard rotation axis To create a Spin shape it is important to know that the green Y axis of the Sketch is the default rotation axis of the Spin shape. When creating a new Spin Shape from scratch using the Spin Wizard you should always use the green axis as the rotation axis. If you have imported a DXF/DWG file into the Sketch, which has the rotation axis of the model drawn in another direction/location than the Y axis, this can be solved in two easy ways; On the image above the rotation axis of the shape follows the red X axis and either needs to be rotated 90 to the green Y axis or; define your own rotation axis with the Center Line tool. Rotate Curves Select all curves and then run the Rotate Curves command. Drag the curves while Drag Entities is active or directly insert the rotation value and then confirm. 18
Create Center Line You can also create your own rotation axis using the Center Line tool, instead of the green Y axis. With a two-click output the line is placed in the Sketch, then Finish the Sketch. Now you can create the Spin shape. A fast way to go is to select the 2D Profile, right click on it and choose Create -> Spin. Fill in the needed changes or just confirm directly. 19
IRONCAD Options, General There are some global settings that affects the Sketch in all files. Remember that most settings are already prepared following the Nefab specific instructions running the CAXA Live Update installer. CAXA Live Update for Nefab IC 2016 settings.rar. Under the Options > Part tab these settings highlighted in red below are good to know about. Mouse pick aperture (pixels) is the area around the mouse cursor that will select something when you left or right click. The camera settings affect how the camera automatically orient itself according to the Sketch plane. Many users turn off the Enable camera Look At during editing, since it will reorient the camera when entering the Sketch. 20
IRONCAD Options, Interaction Under the Options > Interaction tab you will find settings that affect how the geometry updates when dragging handles or in the geometry itself. These settings are highlighted in red below. 21
IRONCAD Options, Color The default colors for the Sketch elements are found under Options > Color. 2D Construction Geometry The default color of 2D construction geometry (curves that does not create geometry) is dark blue. 2D Fully Defined Geometry The default color of 2D fully defined geometry is green. When curves are fully defined they cannot be modified other than through parameters in the parameter table or changes on other geometry that they are defined to. 22
2D Over Defined Geometry The default color of 2D over defined geometry is red. When you add too many constraint relations that IRONCAD cannot possibly solve, a message will appear and the curves will turn red. 2D Over Defined Geometry The default color of 2D under defined geometry is white where under defined means that they are not controlled by any parameters or constraint relations to other geometry. This is the default behavior in IRONCAD and means that it is possible to change the curves in many possible ways. It also makes it possible to work with the Shape handles outside the Sketch. 23
2D profile geometry indicators TRAINING SESSION The default color of 2D profile geometry indicators is dark blue. The indicators can be dynamically turned on and off from the 2D Display toolbar. 2D profile geometry constraint The default color of 2D geometry constraint is red. The indicators can be dynamically turned on and off from the 2D Display toolbar. 2D snap highlight The default color of 2D snap highlight is dark green. The setting to get help from surrounding geometry is called Smart Cursor and can be found when right clicking in the Sketch and choosing Snap. 24
3D Smart Dimensions Highlight TRAINING SESSION The default color of SmartDimensions highlight in 3D (outside the Sketch) is cyan blue, but a darker color like dark blue or black can be visually better. 3D Smart Dimensions and Constraints The default color of SmartDimensions and constraints is cyan blue. A darker color like dark blue, black or red makes Text Annotations and Constraints visually easier to see. 25