Mirroring Pocket

[Murmele]

Hello,

I drawed a sketch and created a pad from it. Next I made some fillets to the pad. Now I would like to mirror the pad, but I'm not able to do that because I get the message: "Please create a subtractive or additive feature first". I found out, that 2016 was the same problem and there it was a packaging problem. Is there a work around for it?

Best regards,

Martin


OS: Linux
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13528 (Git) AppImage
Build type: None
Branch: releases/FreeCAD-0-17
Hash: 5c3f7bf8ec51e2c7187789f7edba71a7aa82a88b
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: German/Germany (de_DE)

[Willem]

Hi Martin, welcome back to Freecad.
The mirrorfunction in the partdesign workbench works different than you expect. It can only mirror pads and pockets in a body and not the total body. For this purpose you should use the mirrorfunction in the Draft workbench. I already did this so you can study your modified file

[Murmele]

Thank you for your help! How can I make pockets into this total body with polar array with 6 times Sketch001?
What is the common workflow to do something like this?

[NormandC]

Hello Martin,

Unfortunately Fillets and Chamfers cannot be patterned in PartDesign.

Here's how to do this in PartDesign:

1. Activate Body
2. Right-click on Pad --> Set tip. This rolls back the Body's history to Pad. Anything that you create next will be added just below the Pad, and above Fillet.
3. Select Pad
4. Create a PartDesign MultiTransform feature with one Mirrored feature on the vertical sketch axis and one Mirrored feature on the horizontal sketch axis. After completing the MultiTransform, set its "Refine" property to "true" to get rid of the residual edges.
5. Select Sketch001 and create a PartDesign Pocket feature.
6. Select Sketch002 and create a second Pocket feature.
7. Select Pocket001 and create a PartDesign PolarPattern feature. In the Pattern parameters, click on Add feature; switch to the Model tab, make Pocket visible; switch again to Tasks tab, click on the Body in the 3D view. You now have Pocket and Pocket001 in the polar pattern. Set occurrences to 6.
8. Right-click on Fillet --> Set tip to return the tip to the bottom.
9. Edit the Fillet and add the required edges by clicking on the "Add ref" button to select one edge at a time. It's slow, but it's the only way.

The Extrude is then useless and can be deleted.

I'll also add that you could design your fillets directly into the Pad sketch.

[Murmele]

Hi NormandC,

great thanks to the great explanation! I tried it another time complete step by step. Thank you!!

[NormandC]

You're welcome.