Drafting a cylindrical face attached to a loft

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pickwick
Posts: 10
Joined: Fri Feb 15, 2019 2:12 am

Drafting a cylindrical face attached to a loft

Postby pickwick » Tue Feb 19, 2019 4:17 am

If I pad a circle, I can select the cylindrical face and then add draft to it, easy as pie.

But if I create a loft, with circular cross sections, and then pad the circle at one end, and try to draft that cylindrical face, I get "Draft Not Possible On Selected Edges/Faces".

Why?


OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.15713 (Git)
Build type: Release
Branch: master
Hash: 93dd00cc3953416bf46fb0a5b7b3c6397df6e4d0
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)
Attachments
Table Leg.FCStd
(27.08 KiB) Downloaded 4 times
Drafted Cylinder Pad.FCStd
(8.5 KiB) Downloaded 3 times
kisolre
Posts: 734
Joined: Wed Nov 21, 2018 1:13 pm

Re: Drafting a cylindrical face attached to a loft

Postby kisolre » Tue Feb 19, 2019 9:01 am

Create Pad by using Sketch and not face of the loft. Add DatumPlane from Sketch. Use it as Neutral Plane for the draft. Reverse direction of the draft.
TableLeg_DatumPlane.JPG
TableLeg_DatumPlane.JPG (84.98 KiB) Viewed 122 times
Attachments
Table Leg_DatumPlane.FCStd
(34.87 KiB) Downloaded 2 times
chrisb
Posts: 15670
Joined: Tue Mar 17, 2015 9:14 am

Re: Drafting a cylindrical face attached to a loft

Postby chrisb » Tue Feb 19, 2019 11:50 am

pickwick wrote:
Tue Feb 19, 2019 4:17 am
Why?
The end of the loft is from the view of the geometric kernel not flat, thus you cannot attach things to it directly.
pickwick
Posts: 10
Joined: Fri Feb 15, 2019 2:12 am

Re: Drafting a cylindrical face attached to a loft

Postby pickwick » Tue Feb 19, 2019 5:17 pm

Not being argumentative, just trying to learn. I understand what both of you are saying, and the datum plane method obviously works. But: you say I can't add directly to the end of the loft, yet my pad is accepted without error. And if I add a second pad on the end of the first pad--just by using the face, not a new sketch--surely that face is flat? (thinking I could add a 1mm pad to the loft, and then add another pad I could draft). And yet I can't draft the cylindrical face of the second pad either.
kisolre
Posts: 734
Joined: Wed Nov 21, 2018 1:13 pm

Re: Drafting a cylindrical face attached to a loft

Postby kisolre » Tue Feb 19, 2019 6:25 pm

pickwick, from here https://www.opencascade.com/doc/occt-7. ... angle.html

Code: Select all

Detailed Description
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This algorithm treats planar, cylindrical and conical faces.
Do not use shapes, which with a draft angle added to a face would modify the topology. This would, for example, involve creation of new vertices, edges or faces, or suppression of existing vertices, edges or faces.
Any face, which is continuous in tangency with the face to be tapered, will also be tapered. These connected faces must also respect the above criteria.
The loft probably defines the final geometry as some splines so despite the fact that the end continues to look like a circle it is not defined as one so it is not a valid surface to draft. When you pad the Sketch the result is a cylinder created from the circle so it can be Draft-ed.
At least that is how I understand it now.
Since there are no limitations mentioned in the PartDesign_Draft Wiki it is hard to realize what is happening.