Hole on pipe wall

[stratosg]

Hi guys again... I have another question for the experts here. On FreeCAD 0.13 I have a pipe wall (two concentric circles padded) and I want to put a whole through that wall. When I select the wall and hit "create sketch" I get a warning "you need a planar face as support for the sketch". I know I'm missing something fundamental here again... Any ideas?

Thanks for the help!

[NormandC]

Hi,

I know I'm missing something fundamental here again...

Actually you're not... The software is!

Part Design is still very young, one of its current limitations is that you can only map a sketch on a planar surface. Which explains why, when you select the cylindrical surface of your pipe, you get the "need planar face as support" warning.

While we wait for Part Design to mature and allow ways of creating features without planar support (quite possibly in v0.14), we've got two workarounds.

1. The simple workaround.
   Create a new part, independent from your pipe, then apply a boolean cut on the pipe. For that do not select a face, and click on the "create sketch" icon, you'll get the plane selection dialog. Then you can pad your sketch, and create the boolean cut. The limitation: you need to set the plane and offset manually, and you cannot use the "copy external geometry" tool. This object will not be associated with your pipe.
2. The creative and convoluted workaround.
   The Part Design workbench expects a planar face for the sketch to map to. So you create one - by building a "temporary feature" that will generate a planar face for your hole. Once the hole is done, you need to cut away the temporary feature. The advantage: fully parametric, all features are associative with the original pipe. The disadvantage: a few more steps than the first method.
   • Typically you would create a sketch on the top face of the pipe. I chose to draw a square with all edges tangent to the pipe's outer cylinder.

     

     FC_pipe-hole-workaround-01.png (8.45 KiB) Viewed 26683 times

   • Then pad it to some arbitrary length, select the front face of the new feature and hit "create sketch".

     

     FC_pipe-hole-workaround-02.png (3.7 KiB) Viewed 26683 times

   • One thing to know: your sketch does not need to lie on the surface of the top block. All that is needed is that the sketch must intersect the whole part, including the pipe. The top block edges can be used as reference geometry to dimension the hole.

     

     FC_pipe-hole-workaround-03.png (10.41 KiB) Viewed 26683 times

     

     FC_pipe-hole-workaround-04.png (4.25 KiB) Viewed 26683 times

   • Now a pocket is applied on the last sketch, creating the desired hole. Now we want to remove the top block, so we select the front face again and create a sketch with a rectangle slightly bigger than the block's face.

     

     FC_pipe-hole-workaround-05.png (19.84 KiB) Viewed 26683 times

   • Finally we apply a pocket, through all, to remove the top block and get our final pipe with hole.

     

     FC_pipe-hole-workaround-06.png (4.89 KiB) Viewed 26683 times

This workaround can be applied to other situations. For example, if you wanted to drill your hole in a slanted way from the pipe, then you could work "sideways", and create a groove (which is a revolve cutout) instead of a pocket.

[stratosg]

Thanks again for an informative reply and all the time you put into making this tutorial (maybe it should go in the wiki?).

I went with the creative method and it worked great

[NormandC]

Glad I could help.

Yes, I think it could be put in the tutorials section. Unfortunately I can't get access to it on weeknights.

[ketilfroyn]

Apologies for waking an old thread, but I use this technique in a basic FreeCAD video tutorial here:

http://www.youtube.com/watch?v=_tyuIIk0M3E&t=12m45s

Just thought I'd add it here in case anyone would want to see a second example.

[Bibi]

The 'artistic' way doesn't work for me, or I do something basic wrong?

My cylinder from a cylinder

freecad.png (154.87 KiB) Viewed 25936 times

I cannot pocket deeper than halfway the base cylinder, I want it all the way through. "Through all" gives me an error as does "dimension" with anything more than the radius of the base cylinder.

[jmaustpc]

Hi Bibi

The 'artistic' way doesn't work for me, or I do something basic wrong?

Please paste a demo file, and your Help about FreeCAD data, then we will be able to work out exactly what is going on in you specific case.

Jim

[Bibi]

Well,.. It became more strange. Whenever I select a face to make a scetch it rotates my part to show another face
I started over and now it seems to be working,... I will be back if I find a similar case. Meanwhile, is there some sort of debug pane, where I can look and find errors in my drawing?

[jmaustpc]

Well,.. It became more strange. Whenever I select a face to make a scetch it rotates my part to show another face
I started over and now it seems to be working,... I will be back if I find a similar case. Meanwhile, is there some sort of debug pane, where I can look and find errors in my drawing?

Depends on what your "Help about FreeCAD data" says.

[Bibi]

You mean the version:

OS: Mac OS X
Word size: 64-bit
Version: 0.14.3703 (Git)
Branch: releases/FreeCAD-0-14
Hash: c6edd47334a3e6f209e493773093db2b9b4f0e40
Python version: 2.7.5
Qt version: 4.8.6
Coin version: 3.1.3
SoQt version: 1.5.0
OCC version: 6.7.0