Comment importer la géométrie de la tôle dans SOLIDWORKS à partir de STEP, Parasolid, IGES, etc.

Importing model geometry can be a real pain if you don’t know how to apply some tricks.  We will take a look at a few techniques for SOLIDWORKS sheet metal import.

Import Geometry

When geometry is imported into SOLIDWORKS, a dialog appears and asks you to run “Import Diagnostics”.

Diagnostics d'importation

We will go ahead and run the SOLIDWORKS Sheet Metal import to see what happens.

It appears that there are 22 faulty faces in the geometry (figure below).  Before we try to repair all errors, we can check where the locations of these errors are.  All the faulty faces seem to be located around the edge flanges on the 4 corners.

Faulty Faces

Now when we look closer, we will find that the flange faces are “coincident” (figure below) by using measure tool.  SolidWorks, or more accurately the ParaSolid kernel it’s built on, does not like “coincident” faces within a single body, that’s why they are treated as faulty faces.  However, there is really nothing wrong with these entities.  We can simply ignore these warnings.

Evaluate Geometry

Now the design tree still has warnings about faulty faces.  We can hide the warnings by going to “Options” -> “System Options” -> “Messages/Errors/Warnings”, and switch “Display FeatureManager tree” to “Never” or “All but top level”.  This is a NEW option introduced in SolidWorks 2012. You will not find it in previous versions. Please see figure below.  Some users prefer leaving these warnings visible, so it is based on your preference.

Messages/Errors/Warning

Transform geometry into Sheet Metal

The next step is to transform the geometry into a real sheet metal part so it can be flatten.  To achieve this, we will utilize the “Insert Bends” command from the Sheet Metal command manager tab.  Notice that there is also “Convert to Sheet Metal” command.  We do not use this command in our case because this command is for when we take a solid “block” model, pick the outer faces to define a sheet metal part.  For more info on this command, please go to “Help” in SolidWorks and search for “Convert to Sheet Metal”.

Insert Bends

When we are in the “Insert Bends” command, pick a fixed face to begin the sheet metal conversion process.  The bend radius only applies for bends with sharp angles.  In our geometry, all bends have round corners since it was an imported sheet metal part.

Insert Bends

After the operation is completed, a good practice is to flatten it and see if everything is fine.  In our model, everything looks great.  If the bends are complex, for instance, edge flanges on curved edges or holes through the bend regions, or if the forming tool applied on the part has “sharp” bends, SOLIDWORKS may see that as an error, or simply remove the feature from the geometry during the “Insert Bends” operation.

Adjust geometry with Move Face

The next operation we will perform is to offset the ventilation hole (for a fan) by some distance.  The command we will utilize is called “Move Face” and found under the “Direct Editing” command manager tab (see below).  Pick the faces as indicated and an edge for direction.  A preview does not show up.  When I click on the check mark to finish, it will actually return with error.  What is going on here?

Move Face

Unfold Bends

Remember earlier I mentioned that SOLIDWORKS does not like “coincident” faces within a single body.  Our sheet metal geometry is still bent during the “Move Face” operation.  To resolve this, we can simply add an “Unfold” command to manually flatten specific bends.  In this case, I will just unfold all bends, and repeat the “Move Face” command.  This time, the preview shows up. Bingo! Clicking the green check mark will finish the command and apply the changes to the model.

Unfold and Move Face

Next, we will move the ventilation holes on another side (see below).  There are hundreds of faces to pick this time.  It is not efficient to add them one by one.  “Box selection” doesn’t seem to pick the hole faces when the orientation is “normal to” the flat.  The trick here is to use either the “Hidden Lines Visible (HLV)” or “Wireframe” display mode.

“Hidden Lines Visible (HLV)” or “Wireframe” display mode

Once the view is toggled, box selection works very well.  This is an odd trick that is not well known. After all faces are selected, we notice that the flat face is also picked. A good practice is to deselect it because we are not moving the flat face.  We are only moving the holes.

Move Face Selections

The “Move Face” command works great now!

If we plan to change the ventilation hole layout, shape, hole count, etc, it may be more efficient to “fill in” the original holes with a simple extrude and then insert a pattern feature as this will provide more control via the pattern parameters.

Hope this article proves useful to you!

En savoir plus sur la tôlerie

Attend a SOLIDWORKS Sheet Metal training course either live online or in a Canadian classroom near you.