TRAINING SESSION Q3 2016

Transcription

1 There are 6 main topics in this training session which is focusing on 3D Import and 2D Drawing Tips and Tricks in IRONCAD. Content 3D modeling kernels D Import... 3 Direct Face Modeling... 5 Unfold smoothly connected faces... 9 Convert to Sheet Metal IRONCAD Drawing Tips and Tricks Tutorial videos: Also remember that we have an English multimedia based training material that you can find on the Nefab Intranet. Day 3 is going through the basics of part and assembly drawings and most of the drawing tools available in IRONCAD. Day 4 has a section where we are looking at the Import of 3D models. IRONCAD ICD Drawing basics playlist (inverted order, 15 down to 1): Import Part 1/3: Import Part 2/3: Import Part 3/3: List of news in v2016 PU1: 4 videos about the Sheet Metal news in v2016 PU1: New unfold in v2016 PU1: Associative Miter in v2016 PU1: Miter Across a Bend: Closed Corner Sheet Metal: 1

2 3D modeling kernels All solid modeling 3D CAD systems are using a solid modeling kernel which defines the way a solid model is built up. The two most common solid modeling kernels are Parasolid (owned by Siemens) and ACIS (owned by Dassault) and are both proprietary licensed by their respectively owners. Both those kernels are used in IRONCAD (one of them is always set as the default) and have been setup to help each other, which means that issues that one kernel might have, might be fixed by the other. This is all working automatically under the hood in IRONCAD, which you as a user seldom or ever take any notice of. This is called kernel collaboration, which is something that IRONCAD is still alone with today, Even though the basic shapes are not really visually different, there are some differences that can be seen visually on two similar parts using the two kernels, when the other kernel doesn t have to help the first kernel to solve how one or many features have an effect on the model and vice versa: One or many parts can manually be switched between the two kernels, either by editing the Part Properties or by using the short cut key command [Ctrl] [K]. The setting is also found in the Property Browser of the selected Part/Assembly or the Scene default settings (when nothing is selected) for the next part created. 2

3 3D Import An imported part only contains a BREP (Boundary REPrepresentation) solid feature of the solid model. In IRONCAD it is still possible to edit a BREP shape with the Triball and shape handles, using a method called Direct Face Modeling, which we will look closer at ahead. It is also possible to convert selected (green) faces into new features listed under the Part in the Scene Browser, such as Blends and Extrudes. There are still not many other 3D CAD systems that can directly edit a BREP shape. File format and solid model issues If the model has been exported using the Parasolid file format (*.x_t) IRONCAD will use Parasolid as the kernel for the imported part. If the model has been exported using the ACIS file format (*.sat) IRONCAD will use ACIS as the kernel for the imported part. This is also true for the native file formats from other 3D CAD systems based on either of the two kernels. The resulting imported part in IRONCAD will be based on the same kernel as the origin program which the native file came from. In that way there are less problems with file translation from other 3D CAD systems to IRONCAD, using the native formats, than there might have been without having two different kernels. The neutral STEP file format uses its own way to define the model, based on the way the default kernel is defining the model. The STEP format is an ISO format and should be the same to and from all systems. But an important thing to remember is that the resulting STEP file doesn t have to be a solid, even if it was modeled as such in the origin program - depending on how the translation between the definition tables are made. It is very common that the translation fails somewhat (or much) and results in a more or less corrupt model, maybe a surface model (which isn t closed ) instead of a solid model, but still a working STEP model. Since the STEP file is a plain text file it is possible to open it in a text editor and read which origin program that created the file was, in the header of the STEP file. In that way you can see that the other program, based on maybe the Parasolid kernel, was the origin and if you can get a Parasolid *.x_t file instead the import will probably be working better. Parasolid and ACIS can also interpret the STEP model with different results after import. In that way it is important to do a new import using the other kernel, if the first import fails, when the reason might be the origin program being based on the other kernel. 3

4 This is also why you should make sure that the import setting Run statistics after import is active. It will control the model for any inconsistencies and show a result after the import is done. Based on the result you can make sure that the model is working fine, which might include more or less work depending on the nature of the issue. The control can also be run manually on any part or assembly, by first selecting the object to check and then run the Statistics button under the Tools ribbon tab or the Tools menu. 4

5 Direct Face Modeling It is possible to edit an imported BREP shape in IRONCAD using a method called Direct Face Modeling (DFM). The changes won t add more features in the Part history, only change the lump of geometry of the BREP shape. In that way no unnecessary history must be created, which could intervene with now unknown future changes. Every change is completely independent of what happened earlier. Move Face Select a face and turn on the Triball to move the face or right click on the selected face to get a menu. The Triball activation on a face will start the Move Face command (or when Move is chosen from the face menu). Use the Triball options to move to the desired location. It is also possible to create a copy of the hole (face) by selecting Copy Feature in the Command Browser. 5

6 Edit Face Radius TRAINING SESSION It is possible to edit the radius of a face, without having to measure the radius first or creating a new feature from it, keeping the simple geometry simple. Select the face and choose Edit Face Radius from the right click menu of the face. In the Property Browser the current Radius value is shown and can be edited. By enabling the Auto Face Grouping option all faces with the same properties are automatically selected and edited. Faces to Intellishape It is also possible to create a feature from a face selection, such as a hole or a blend by selecting the Faces to Intellishape option on the face menu. To make it easier to select all faces that might be needed, use the Selection Filter and choose Faces by auto-feature, then select a face. Depending on which face that is chosen within that group of faces, the resulting selection might be different. 6

7 Now when all faces in the feature has been selected, right click on one of them and choose Faces to Intellishape. In this specific case a new extrude feature is created, visible under the Part in the Scene Browser. Now, since the selection had 4 rounded corners, which have been converted into arcs in the extrude Sketch, the Shape handles cannot be used to extend the length of the rectangle shape. This is a common problem, but can easily be solved. By editing the Sketch of the extrude and replacing the arcs with fillets instead, the Shape handles will now be working as expected. This is easily tested by dragging the curves in the Sketch, if they follow along, the Shape handles will be working as well. 7

8 The right click options of the Shape handles can now be used to set dimensions to other geometry. Thicken Shape Faces can also be used to create new parts, based on the selected faces. Select the faces and right click on any of them, choose Create -> Thicken Shape. In the Property Browser the settings for the new part is controlled; Thickness and Direction. The new part is added and also contains a simple BREP shape. 8

9 Unfold smoothly connected faces With the tool Solid/Surface Flat Pattern from Faces any model that has faces that are smoothly connected can be unfolded into a new part. When the tool is started, two steps are the minimum requirement. 1) Decide which thickness to use, either from the Standard Stock where you select another thickness from the Change Stock option or by reading it from the imported model, by selecting Custom Stock. 2) Select a face from the imported model. All smoothly connected faces will automatically be added to the selection. When the tool is finished a new unfolded part is created. The BREP shape of the new part also contains the Bend Line Information; angle, radius and direction, which can be transferred to the drawing. 9

10 Convert to Sheet Metal An imported model that can be unfolded can also be converted into a new Sheet Metal part in IRONCAD from version 2016 PU1. The new part will be based on the specific features needed to build a Sheet Metal part, first an extrude with the unfolded outline, then the new Sketched Bend feature, which creates bend features from single curves in a sketch. To convert an imported part, use the Convert to Sheetmetal part tool under the Sheet Metal ribbon tab. For the Toolbar interface the Convert to Sheet Metal Part button must be manually added first, by going to the Customize Toolbar/Menu/Keyboard under the Command tab you will find the icon under the category All Commands, then drag and drop the icon from the Commands list to the toolbar. 10

11 When the tool is started, two steps are the minimum requirement. 3) Decide which thickness to use, either from the Standard Stock where you select another thickness from the Change Stock option or by reading it from the imported model, by selecting Custom Stock. 4) Select a face from the imported model. All smoothly connected faces will automatically be added to the selection. When the tool is finished a new Sheet Metal part is created. Possible issues In the model used as an example here there s a problem with the Sketched Bend feature, which gets double lines on two places, due to the shape of the imported model (the issue is known and will be fixed in a future update). This is easily fixed manually as well though, by editing the Sketch Curves of the Sketched Bend and removing the extra lines. 11

12 By looking in the Scene Browser under the Part the Sketched Bend feature is shown with an extra red crossed issue icon. Right click on the Sketched Bend feature and choose Edit Sketch. Remove all double lines and then Finish the Sketch. The Sketched Bend feature is now working properly and the Part looks correct. 12

13 One reason to convert an imported model into a Sheet Metal part is that new Sheet Metal features can be unfolded, which creates a new configuration which can be projected on a 2D drawing. If the folded Sheet Metal part changes the unfolded part can be updated and the drawing automatically reflects those changes. Another reason to use the Convert to Sheet Metal Part tool is to add new Sheet Metal features from the Sheet Metal catalog, such as a Bend feature. It is not possible to drop any Sheet Metal feature on an imported model. 13

14 Face to DXF TRAINING SESSION IronPRO XT has a tool called Face to DXF which creates a DXF file from the face the tool is dropped on. The name is suggested from the Part Name in the Scene Browser. Save the file to a folder and choose which DXF version to use. When the export is finished the result is shown in a new window: There are currently some limitations regarding certain spline, arc and elliptic arc geometries in the Face to DXF tool. Always check the resulting file after export. If it has gaps or strange looking arcs it might be because of the current limitations. If so, create a new 2D drawing and export it to a DXF file instead. Known limitations in the IC API used by the Face to DXF tool: CURVE2D_FILLET CURVE3D_ELLIPTICALARC CURVE3D_INTERPOLATION_SPLINE Z_CURVE3D_BSPLINE 14

15 IRONCAD Drawing Tips and Tricks The IRONCAD Drawing (ICD) is mainly used for projecting 3D models from different preset views. There are some news regarding view placement in version 2016 PU1 and also some common unknown Tips and Tricks regarding the dimension tools that we ll have a look at here. Create Views To create a new set of views, click on the Create Standard View button under the View tab or Standard toolbar. The default direction of the preview image uses Y up, X to the right and Z against you, compared with the 3D scene you are working with. If this isn t what you want you can either rotate the view with the buttons or go back to 3D and rotate or use the Look At tool to get another angle, then use the From Scene button at the bottom left. The view content will not change if you rotate the models in the 3D scene afterwards, only if you go back to the view orientation settings and press the From Scene button again. If the default View Creation Mode of the template (an option in the Drawing Browser) is set to Precise Mode, there s no support for Shaded Rendered views. If you have some parts with a transparent setting, they are best shown when using Quick Mode. A new setting in version 2016 PU1 is the Auto place dependent views at the bottom of the window. With it Off you will be able to place each view independently, instead of all of them at once, when you finish the Standard Views Creation window by pressing OK. When placing the views, use the keyboard up/down arrow keys to adjust the view scale before placing them on the sheet. The red view border will preview the scale change. 15

16 Place dimensions TRAINING SESSION Dimensions are created by using one of several dimensioning tools. The SmartDimension tool is a combination of Linear (horizontal/vertical), Radius, Diameter and Angle dimensions in one tool, depending on where and how you click. A general rule in 3D CAD is to try to avoid using a vertex/point for dimensions, if possible. The main reason is that a point might move in an unexpected direction or even disappear (replaced by a chamfer or blend feature), making the dimension not only having to update but also take a decision -> where to go now?. Any point close by might be the new reference for the dimension. Instead you should set dimensions from and to edges, which are much more reliable over time. To set a dimension from an edge, hold down the [Shift] key and click on the edge, then release the [Shift] key for the second click. The [Shift] key will tell the program; instead of reading the values from the edge (length or radius/diameter), create a reference from the edge. When the reference ([Shift]) click is made from a circle or an arc, there will also be an Arc Option added under the Linear Dimension Properties, where the dimension extension line can be moved from the circle/arc center to the minimum or maximum values of the circle. When placing a new SmartDimension you can also snap the dimension in height with any other already existing dimension. Just move the mouse cursor and snap to the other dimension. 16

17 As an example, all these ten dimensions below have been placed using the SmartDimension tool, by holding down the [Shift] key on the first click of a hole circle. By pressing [TAB] or right click during placement, the orientation of the dimension will switch between Parallel, Horizontal and Vertical. The setting of some of the dimensions below has also been altered, to take the hole radius in consideration for placement of the Dimension Extension Line, which will of course affect the dimension value. Under the right click menu and Properties of a dimension there are Arc Options shown under the Dimensions tab, where these settings are controlled. The Minimum and Maximum options will remove or add the radius value to/from the Center, for the Dimension Extension Line. 17