FreeCAD model does not work upon revision

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!
User avatar
YCStone_
Posts: 26
Joined: Fri May 06, 2016 3:10 am
Location: Xiamen - CHINA
Contact:

FreeCAD model does not work upon revision

Postby YCStone_ » Tue Jul 05, 2016 12:13 pm

hello,
i would like to ask some help why in the modelization in FreeCAD , it is very hard to modify the objects
for example i have an object which has surface curve on both sides of the rectangular box, when i tried to make modification on the surface curve , for example the radius of the curve, all the child coming from this curve does not work anymore, it means that you have to redo again from the point where you make the curve. so imagine productivity waste on our part when we use FreeCAD.
i will send the drawing to indicate my point on this later. but pls can anyone inform us on how to handle this issue
thanks a lot so much
best regards
YC Stone
xiamen china
YC Stone Natural Stone Supplier
User avatar
yorik
Site Admin
Posts: 11840
Joined: Tue Feb 17, 2009 9:16 pm
Location: São Paulo, Brazil
Contact:

Re: FreeCAD model does not work upon revision

Postby yorik » Tue Jul 05, 2016 9:34 pm

Hi,
You are definitely doing something wrong... The whole point of FreeCAD is to be parametric, and therefore make it easy to do that kind of things: Change one curve and not have to rebuild the whole model.
Yes, please attach your file, we might be able to tell you what is wrong.
User avatar
NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: FreeCAD model does not work upon revision

Postby NormandC » Wed Jul 06, 2016 2:55 am

yorik wrote:You are definitely doing something wrong...
Is he/she?

How about the well known topological naming problem? YC Stone's description is as good as any of this crippling issue at the heart of what aims to be a parametric program.
User avatar
bejant
Posts: 6076
Joined: Thu Jul 11, 2013 3:06 pm

Re: FreeCAD model does not work upon revision

Postby bejant » Wed Jul 06, 2016 10:31 am

YCStone_ wrote: imagine productivity waste on our part when we use FreeCAD.
Yes, it's a known problem.
YCStone_ wrote:i will send the drawing to indicate my point on this later. but pls can anyone inform us on how to handle this issue
The FreeCAD .fcstd file will help us see what exactly is going on, but I also suspect that your problem is because changing the curve changes the number of faces and edges (that's the topological naming that NormandC mentioned). One option is to create your Sketches in the 3D space without attaching them to a face, and then use Part WB > Booleans (Fusion, Cut, and so on) instead of Part Design WB > Pad, Pocket, etc. where the Sketches are attached to faces.
User avatar
YCStone_
Posts: 26
Joined: Fri May 06, 2016 3:10 am
Location: Xiamen - CHINA
Contact:

Re: FreeCAD model does not work upon revision

Postby YCStone_ » Wed Jul 06, 2016 11:20 am

thanks for the reply
The FreeCAD .fcstd file will help us see what exactly is going on, but I also suspect that your problem is because changing the curve changes the number of faces and edges (that's the topological naming that NormandC mentioned).
you are definitely correct i change the number of sides of the curve, from a 3 line2 and a curve to 4lines and curve, this is what we usually do. always the design is changing. and probably many more additional curves for edit. so if i really what to make the changes like this on the curve, parametric freecad will fail? so it it means i have to do it again from the point where the change curve effected? so this is inherent in freecad?
One option is to create your Sketches in the 3D space without attaching them to a face, and then use Part WB > Booleans (Fusion, Cut, and so on) instead of Part Design WB > Pad, Pocket, etc. where the Sketches are attached to faces.
yes i know this solution, but the sketcher has a very strong functionality where you can create an edge-linked with the geometry of an object. in solidworks you can have edge-linked on any plane and bodies - very good time saver to find the reference line, but in freecad what we got is for the sketcher only, besides it is limited only to the plane on that surface. so my point is i like sketcher, i got productivity boost using sketcher because of edge-linked. if there is not other way, then we just have to do on what we have for the moment.
YC Stone Natural Stone Supplier
User avatar
YCStone_
Posts: 26
Joined: Fri May 06, 2016 3:10 am
Location: Xiamen - CHINA
Contact:

Re: FreeCAD model does not work upon revision

Postby YCStone_ » Wed Jul 06, 2016 11:34 am

thanks for all the reply

pls find the attached file
i got a problem file:
problem_try_to_pocket_the_sketch.fcstd
(8.04 KiB) Downloaded 16 times
where i have a box.
then i cut a curve from the box using sketch(1st sketch), then i cut again the box again on the other using another sketch(2nd sketch).
i like the sketch because it permits me to get the edge of the box, then i can have perpendicular constraints on that edge.
so far so good.
then i make changes to first sketch, the changes are just simple additional lines and curves, after that update then the cut from the 2nd sketch did not work now, i tried to edit the 2nd sketch freecad would not permit, only says error.


the second file is the solution, where i erase the first sketch and all its childe and try to make a new cut from the surface of the 2nd sketch cutout all over again.
solution_recreate_the_sketch_all_over_again.fcstd
(11.68 KiB) Downloaded 16 times
so i really got low efficiency here.

also it happens but not in this file that i got a broken face even after i recreate the sketch again.
my point in telling this is not to complain, its only i encounter a problem and if there is a solution, if none then we just have to do what we have for the moment, until succeeding version got updated
thanks a lot so much!

pls find my ubuntu setup below
OS: Ubuntu 15.10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6703 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.10
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
YC Stone Natural Stone Supplier
User avatar
bejant
Posts: 6076
Joined: Thu Jul 11, 2013 3:06 pm

Re: FreeCAD model does not work upon revision

Postby bejant » Wed Jul 06, 2016 5:56 pm

YCStone_ wrote:thanks for all the reply

pls find the attached file
i got a problem file:

problem_try_to_pocket_the_sketch.fcstd
(8.04 KiB) Downloaded 2 times


where i have a box.
You have another problem going on in that file. When you made the Sketch, and then the first Pocket, you should have left Pocket visible and left Cube hidden. Instead you went back and selected another face of Cube and created another Sketch. That forked your model:
20160706a.png
20160706a.png (10.65 KiB) Viewed 1105 times
You should have Mapped one of your Sketches onto a face of "Pocket" instead of onto "Cube".
20160706b.png
20160706b.png (17.6 KiB) Viewed 1104 times
And i see from that last image it looks like I should have used the Reorient Sketch tool instead of Map Sketch To Face tool because there are still two dependencies to Cube.
pocketed_sketch.fcstd
(16.72 KiB) Downloaded 15 times
OS: Ubuntu 14.04.4 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6703 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

Let me have a better look at this and I'll post back. Maybe the Spreadsheet WB might be good to use here.
User avatar
bejant
Posts: 6076
Joined: Thu Jul 11, 2013 3:06 pm

Re: FreeCAD model does not work upon revision

Postby bejant » Wed Jul 06, 2016 11:54 pm

YCStone_ wrote:so i really got low efficiency here.
If you made your Sketch geometry a little differently, you could have avoided a lot of the problems that happen when you change the curves later. In looking at the Sketches I see that only the curves cross the face of your object:
2016070c.png
2016070c.png (10.72 KiB) Viewed 1092 times
It looks like you could arrive a simpler valid result instead by using only one circle for each Sketch, and often times the simpler you can make your model the better it will be.
User avatar
NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: FreeCAD model does not work upon revision

Postby NormandC » Thu Jul 07, 2016 12:14 am

YCStone_ wrote:so this is inherent in freecad?
It's inherent to the geometric modeling kernel that FreeCAD uses. The modeling kernel is the software library responsible for making geometry operations, it's called Open CasCade and the FreeCAD developers have no control over its development.

The problem is that internally, when an object is edited, the topology (edges, faces) gets renumbered differently. This is why after some edits (not all) sketches switch faces unexpectedly, fillets or chamfers fail or get switched to a different edge, etc.

One FreeCAD developer is currently working to try to workaround this problem in FreeCAD, but it's very complex and nobody knows when (or even if) it's going to be completed.
User avatar
NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: FreeCAD model does not work upon revision

Postby NormandC » Thu Jul 07, 2016 12:24 am

bejant wrote:often times the simpler you can make your model the better it will be.
Honestly, this shape should be done from one sketch and one pad, that's it. This would not suffer from failed edits.
FC_YCStone_sample_01.png
FC_YCStone_sample_01.png (42.64 KiB) Viewed 1088 times
But I'm guessing this was just an example file.