PartDesign: pad up to face

Post here for help on using FreeCAD's graphical user interface (GUI).
Forum rules
and Helpful information
IMPORTANT: Please click here and read this first, before asking for help

Also, be nice to others! Read the FreeCAD code of conduct!
Post Reply
emills2
Posts: 868
Joined: Tue Apr 28, 2015 11:23 pm

PartDesign: pad up to face

Post by emills2 »

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 2108 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 2108 times
so if my 0 height issue is related to supports, how can i get my datum plane 'into the support'?
TheMarkster
Veteran
Posts: 5505
Joined: Thu Apr 05, 2018 1:53 am

Re: PartDesign: pad up to face

Post by TheMarkster »

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: 868
Joined: Tue Apr 28, 2015 11:23 pm

Re: PartDesign: pad up to face

Post by emills2 »

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 2100 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 36 times
TheMarkster
Veteran
Posts: 5505
Joined: Thu Apr 05, 2018 1:53 am

Re: PartDesign: pad up to face

Post by TheMarkster »

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 2097 times
Attachments
first_pad_to_datum(2).FCStd
(7.93 KiB) Downloaded 36 times
User avatar
NormandC
Veteran
Posts: 18587
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: PartDesign: pad up to face

Post by NormandC »

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: 868
Joined: Tue Apr 28, 2015 11:23 pm

Re: PartDesign: pad up to face

Post by emills2 »

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
Founder
Posts: 20241
Joined: Thu Feb 19, 2009 10:32 am
Contact:

Re: PartDesign: pad up to face

Post by wmayer »

The bug is fixed with git commit fe2660b46 and was part of issue #0003177
User avatar
NormandC
Veteran
Posts: 18587
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: PartDesign: pad up to face

Post by NormandC »

The parallel to sketch plane limitation was not, we discussed it in another topic... I'll try to find it.
chrisb
Veteran
Posts: 53919
Joined: Tue Mar 17, 2015 9:14 am

Re: PartDesign: pad up to face

Post by chrisb »

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
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
Post Reply