Recognize a dead solid in CATIA Sheet Metal
This video is split in 2 parts:
1) Design of the part in CATIA Part Design. (0:14 to 7:22)
2) Recognition of the Dead Solid plate in Sheetmetal. (7:22 to 10:40)
You will see that you can transform a dead solid into a Sheet metal part. The algorithm recognize the manufacturing processed shape, such as bending, boss, hole, etc. You will be able to unfold/fold the part and make a drawing generating the unfolding lines.
Step 1: Video
Step 2: Create a fictional plate
Create a new Part in Part Design
Sketch a non closed profile
Create a solid using the feature Pad with the option "Thick"
-> use the option neutral fiber and put 2mm in value.
Add 2mm fillet on the inner corner and 4mm fillter on the outer corner
* This should look like a sheetmetal plate, but it is only a solid part *
Continue your design by adding other sketch profile perpendicular to first sketch
Add holes, bosses, chamfer, etc.
* Make it similar to a plate AND keep the same thickness all the time AND use fillets 2mm/4mm *
Step 3: Transform the part in a dead solid
* Now you part looks like a plate, you will transform it to a dead solid *
Create another part in Part Design (with different name)
In the first part, right click on the PartBody and select copy
Switch to the new part, right click on the 3DShape and select "Paste Special"
A panel appears, select "As Result"
* You will have a dead solid now *
Step 4: Recognize the sheetmetal
Keep the part open, but switch to Sheet Metal Design Application
Click on Sheet Metal Parameters
- Thickness = 2mm
- Bend Radius = 4mm (Or if you have a bigger fillet in your part, like in the video R10mm, put the biggest value)
Click on the Recognize feature
Select the dead solid
Select a face that will be the support when part is flatten
(optional) you can do a manual recognition if the automatic recognition does not allows you to unfold the part
Click on OK
* Your part is now consider a a sheet metal part and can be unfolded *
Step 5: Unfolded view in drawing (option)
Insert a drawing in the 3DPart
Go to drafting application
Create normal views (front, side, top)
Expand the action bar (click on small arrow ">")
Select the unfold view
Switch back to the sheet metal part and click on it
* the view will be generated on the drawing and the bending lines should also appears in the view *
- End of tutorial