How to remove dependency from import?

[amunizp]

Data
OS: Ubuntu 16.04.3 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6712 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: da2d364457257a7a8c6fb2137cea12c45becd71a
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
File under discussion:

VacuumFormORiginal.fcstd

(227.67 KiB) Downloaded 25 times

My intention
Use an existing model to create an STL file of the "filling" of the sample. This is to be used in a vacuum former.
What I did:
Imported a STEP file into FreeCAD.
Using the Part design I fitted the sketch the best I could to the inside of the model. Curved features were done by hand using a couple of ellipses as I could not use edge linked.
Paded the sketch
Hid [SPACE] the original imported step file, selected the new pad and followed instructions here to export only the new pad.
What I got was the full model.
I read items on this forum [1] and [2] but I don't think they are the same issue.
I have tried deleting the original imported figure even assuming the complaining of the links but the original imported model is still there.
I have tried coping the sketch from one file to another file but simple copy and paste does not seem to work.

Screenshot from 2017-09-20 11-18-43.png (146.91 KiB) Viewed 1620 times

The ask
Did I follow a correct work flow?
Should I do something differently?

[bejant]

Hi amunizp, and welcome! You want to Export only Pad. Did you select everything (or use Crtl + A) by mistake?

Edit: Scratch that, I see there is something odd going on in your model. Let me look at it some more and I'll post back in a few minutes.

[bejant]

I don't know why the .step portion wants to Pad too.

Open the file and save it as another name.
Delete the .step thing from your file.
Delete Pad.
Select the Sketch, then click the Pad tool.
Enter a length of 312 mm, tick the Reversed tick-box to True, and click the Ok button.

20170920a-016-VacuumForm.fcstd

(17.42 KiB) Downloaded 36 times

I hope you now have half of your form. Use Part WB (not Part Design) > Mirror to create the other half, then use Part WB > Fusion to make a Fusion of the two halves.

OS: Ubuntu 16.04.3 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6712 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: da2d364457257a7a8c6fb2137cea12c45becd71a
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[amunizp]

I don't know why the .step portion wants to Pad too.

Thanks for having me!

Could it be that the sketch as links to it? I used the "create an edge linked" maybe it linked a bit too much.

Quick question, what other method would you would have used? I really want to get the rounded edge right, current fit is close but not exactly.

• I also tried drawing a rectangular sketch to XY plane and extruding to face but the step file has a couple of faces, so maybe meshing it first?

• Also I could not find how to link the edges to the sketch to get the right size.

• Is there a way to break the STEP into surfaces and then essentially but walls on the structure and mesh the full body?

• Maybe extrude from the surface to the XY plane?

Open the file and save it as another name.
Delete the .step thing from your file.
Delete Pad.
Select the Sketch, then click the Pad tool.
Enter a length of 312 mm, tick the Reversed tick-box to True, and click the Ok button.

20170920a-016-VacuumForm.fcstd

I hope you now have half of your form. Use Part WB (not Part Design) > Mirror to create the other half, then use Part WB > Fusion to make a Fusion of the two halves.

This worked. Thank you very much, I was struggling for hours on this. Why not the mirror on part design?

[NormandC]

Hello amunizp,

Could it be that the sketch as links to it? I used the "create an edge linked" maybe it linked a bit too much.

Actually, if you mapped the sketch to the imported STEP, it's normal that a PartDesign Pad would combine with the underlying solid, that's the way the PartDesign workbench works.

If you want to map a sketch to an existing solid (to use external geometry), but want to create a separate solid, then you should create a Part Extrude instead.

Curved features were done by hand using a couple of ellipses as I could not use edge linked.

That's because at the moment, only straight edges and arcs are supported. The Sketcher should have told you as such if you have the Report view open (enable it from the View --> Panels menu).

so maybe meshing it first?

Meshing is not useful in CAD, apart from FEM analysis or export for 3D printing.

Is there a way to break the STEP into surfaces

Yes, you can use Draft Downgrade to "explode" the solid into faces. But this work flow would be time consuming, the STEP solid has holes and rounded corners, so you couldn't reuse the exploded faces to construct a new solid for your mold.

Here's one method to build the mold imprint using the exact inner 2D section of your imported STEP solid. The general principle is

1. Extract the inner 2D section of the imported solid (parallel to XZ plane)
2. Close it with a bottom horizontal edge to form a Wire, then upgrade it to a face
3. Extrude the face

It's a little more involved than that with your model, not sure why exactly.

What I did step by step:

1. Centre the imported solid in reference to the XZ plane (not obligatory but I prefer to have my models centred on the origin )
2. Cut ( Part Cut) the imported solid with a Pad that meets the XZ plane. I could have use a simple primitive Cube instead, but I prefer to work with sketches.
3. The resulting cut solid now has a side lying on the XZ plane with no rounded corners:

   

   FC_amunizp_mold_01.png (13.22 KiB) Viewed 1585 times

4. Switch to the Draft workbench, select the inner faces of the Cut object and create a Draft Facebinder. This creates a new "Facebinder object that copies all the inner faces, so we no longer have a thickness.
5. Switch to the front view (1 key on the keyboard).
6. Select the Facebinder and create a Draft Shape2DView. This creates a linked Shape2DView profile of the Shapebinder, but it creates it on the XY plane.

   

   FC_amunizp_mold_02.png (12.67 KiB) Viewed 1585 times

7. Use Edit --> Placement to rotate the Shape2DView object to the XZ plane. I recommend you check "Apply incremental changes to placement", this will be a lot more intuitive. First apply a 270 degree (-90) rotation in Z axis, then a 90 degree rotation on the X axis.
8. Hide everything but the Shape2DView object.
9. Draw a Draft Line between the end points of the Shape2DView. In the Draft Snap toolbar, make sure the end point snap is enabled and that the "Restrict to working plane" icon is disabled.
10. Now, in theory, it would just be a matter of selecting both the Shape2DView and the Line and apply Draft Upgrade to join them into a Wire. Unfortunately it doesn't work. So we need to look into this further.
11. Select Draft2DView and click on Draft Downgrade once to reduce it to a non-parametric shape (its icon in the Model tree will turn into a blue cube), then a second time to explode it into its separate edges.
12. And now we see the problem: there are 23 edges, which is way too many! By selecting one after the other, we can see that many segments overlap and thus prevent the creation of a closed wire. Some of them fail to be displayed in the 3D view. We need to clean these edges up, and delete all the ones that are superfluous. Only 5 contiguous edges should be left.

    

    FC_amunizp_mold_03.png (3.61 KiB) Viewed 1585 times

13. Select the 5 edges and the Line, then click on Draft Upgrade once to create a Wire, then a second time to upgrade the Wire into a Face.

    

    FC_amunizp_mold_04.png (3.21 KiB) Viewed 1585 times

14. Next switch to the Part workbench, select the Face and click on Part Extrude. Set its direction to Y, and its length to 312 mm.

    

    FC_amunizp_mold_05.png (14.58 KiB) Viewed 1585 times

And you're done.