PartDesign: pad up to face

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emills2
Posts: 577
Joined: Tue Apr 28, 2015 11:23 pm

PartDesign: pad up to face

Postby emills2 » Sun Oct 28, 2018 10:32 pm

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13541 (Git)
Build type: Release
Branch: releases/FreeCAD-0-17
Hash: 9948ee4f1570df9216862a79705afb367b2c6ffb
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)

i want to pad the first solid from a sketch up to a datum plane. the tool complains about 0 height even though the datum plane and sketch plane are not equal.
pad_up_to_datum_plane.PNG
pad_up_to_datum_plane.PNG (67.35 KiB) Viewed 365 times
i didn't see anything that seems to relate to my situation on the wiki, except a comment about supports, but the "support" concept is not explicitly defined (or linked to a definition)
pad_support_undefined.PNG
pad_support_undefined.PNG (97.71 KiB) Viewed 365 times
so if my 0 height issue is related to supports, how can i get my datum plane 'into the support'?
TheMarkster
Posts: 1061
Joined: Thu Apr 05, 2018 1:53 am

Re: PartDesign: pad up to face

Postby TheMarkster » Sun Oct 28, 2018 10:47 pm

I believe there was a fix not too long ago for the 0 height issue when padding up to a face, but I don't know if it was applied to 0.17. You could try your model with one of the 0.18 builds.
emills2
Posts: 577
Joined: Tue Apr 28, 2015 11:23 pm

Re: PartDesign: pad up to face

Postby emills2 » Sun Oct 28, 2018 10:54 pm

here is an interesting experiment:
-datum plane on body's XY, no offset
-sketch on datum plane
-datum plane on sketch, add offset
-pad sketch to second datum plane

produces an object, but padded in opposite direction, at a random length
datum_to_datum_weird_result.PNG
datum_to_datum_weird_result.PNG (105.88 KiB) Viewed 357 times
now that i think about it, it seems the wiki says you cannot pad up to a face unless it is already part of your object:
"If there is no support, no selections will be accepted."
why not? i want to start my body by padding between two predefined planes. Because i specifically want to to be able to track those faces, and sketch on them as datum planes, not as body faces to avoid topological messes.

is this intentionally forbidden? and if it must be forbidden, why can't the datum planes be considered part of the support?
Attachments
first_pad_to_datum.FCStd
(15.92 KiB) Downloaded 5 times
TheMarkster
Posts: 1061
Joined: Thu Apr 05, 2018 1:53 am

Re: PartDesign: pad up to face

Postby TheMarkster » Sun Oct 28, 2018 11:21 pm

DatumPlane001 is attached to Sketch. Maybe that's the problem? In the attached model I have attached both datum planes to the xy plane and it seems to work as expected.
datumplanes.png
datumplanes.png (21.95 KiB) Viewed 354 times
Attachments
first_pad_to_datum(2).FCStd
(7.93 KiB) Downloaded 4 times
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NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: PartDesign: pad up to face

Postby NormandC » Sun Oct 28, 2018 11:38 pm

emills2 wrote:
Sun Oct 28, 2018 10:54 pm
is this intentionally forbidden?
I'm pretty sure it's not, only an oversight. Another arbitrary limitation is that the datum plane needs to be parallel to the sketch plane. This was discussed some time ago with wmayer.

The PartDesign Pad wiki page needs to be updated, padding the first base feature up to a datum plane was only added in v0.18, with the limitation I mention above, and which I hope can be lifted before the 0.18 release.
emills2
Posts: 577
Joined: Tue Apr 28, 2015 11:23 pm

Re: PartDesign: pad up to face

Postby emills2 » Mon Oct 29, 2018 12:56 am

TheMarkster wrote:
Sun Oct 28, 2018 11:21 pm
DatumPlane001 is attached to Sketch. Maybe that's the problem? In the attached model I have attached both datum planes to the xy plane and it seems to work as expected.
thanks TheMarkster. is your model in 0.18? (fyi, i tried attaching the second datum plane in various ways and it didn't help me)
NormandC wrote:
Sun Oct 28, 2018 11:38 pm
The PartDesign Pad wiki page needs to be updated, padding the first base feature up to a datum plane was only added in v0.18, with the limitation I mention above, and which I hope can be lifted before the 0.18 release.
Thanks NormandC
wmayer
Site Admin
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Re: PartDesign: pad up to face

Postby wmayer » Mon Oct 29, 2018 8:57 am

The bug is fixed with git commit fe2660b46 and was part of issue #0003177
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NormandC
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Location: Québec, Canada

Re: PartDesign: pad up to face

Postby NormandC » Tue Oct 30, 2018 3:35 am

The parallel to sketch plane limitation was not, we discussed it in another topic... I'll try to find it.
chrisb
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Joined: Tue Mar 17, 2015 9:14 am

Re: PartDesign: pad up to face

Postby chrisb » Tue Oct 30, 2018 6:51 am

NormandC wrote:
Tue Oct 30, 2018 3:35 am
The parallel to sketch plane limitation was not, we discussed it in another topic... I'll try to find it.
You wrote about it in the tracker of issue #3177