Chamfering difficulties

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un1corn
Posts: 155
Joined: Sat Dec 26, 2015 2:06 pm

Chamfering difficulties

Postby un1corn » Fri Mar 04, 2016 1:07 pm

Hello Everyone.
I am seeking guidance on a problem that I have, Briefly as a learning curve I am drawing the parts of a model Lanzing Bulldog vehicle.
I have created the attached worm screw but I am unable to chamfer the ends to achieve the appearance in the drawing (JPG of the worm screw drawing also attached) the chamfer also chamfers the end of the thread indicated by arrow.
I have extended the thread profile inwards by 0.1mm the ensure no gaps between the inner cylinder and thread form.
If I create a fusion to try a chamfer all sort of weird things occur, I am sure that it is my lack of experience causing these problems.
I would appreciate help with this if possible please.
Thanks in advance.

OS: Windows 8 (Upgraded to 10)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4671 (Git)
Branch: releases/FreeCAD-0-15
Hash: 244b3aef360841646cbfe80a1b225c8b39c8380c
Python version: 2.7.8
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
Attachments
Worm Screw.JPG
Worm Screw.JPG (27.87 KiB) Viewed 1429 times
worm gear screw original.FCStd
(253.82 KiB) Downloaded 21 times
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tanderson69
Posts: 1530
Joined: Thu Feb 18, 2010 1:07 am

Re: Chamfering difficulties

Postby tanderson69 » Fri Mar 04, 2016 2:51 pm

I am on a different version of occt, so we probably have a different experience. When I open your part and run part/check geometry, I get a lot of errors. If you have errors from part/check geometry then you should track down where these errors are created. In case you didn't know, you should get into the habit of checking your model periodically through construction, especially when dealing with models using loft and sweep. Try to fix errors as they occur. I did a full recompute and got a error-free model. I am sure this is because I am on occt 6.9.1. After that I was able to build subtraction solid from a cube and a cone that will put a 'chamfer' on the end. I wouldn't expect the chamfer feature to do what you want in that condition.
mario52
Posts: 2921
Joined: Wed May 16, 2012 2:13 pm

Re: Chamfering difficulties

Postby mario52 » Fri Mar 04, 2016 3:32 pm

hi
see here one example

help - trapezoidal lead screw

mario
Maybe you need a special feature, go into Macros_recipes and Code_snippets, Dialog creation. My macros on Gist.github.
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bejant
Posts: 6076
Joined: Thu Jul 11, 2013 3:06 pm

Re: Chamfering difficulties

Postby bejant » Fri Mar 04, 2016 4:48 pm

un1corn wrote:If I create a fusion to try a chamfer all sort of weird things occur, I am sure that it is my lack of experience causing these problems.
I don't think it's possible to Chamfer your model as it is now. The CAD kernel can't deal with where your threads meet the cylinder.

Also, Fusion fails Check Geometry with BOPCheck enabled. This can be easily fixed by using the Placement property to rotate the cylinder a little bit about the Z Axis so that the seam of the cylinder doesn't line up with the seams of the Sweep. I rotated the cylinder 10 degrees, and then Fusion was valid.

But cutting threads works better for me than adding them, so I used a different approach (probably pretty close to what Mario linked to):
20160304a-worm.png
20160304a-worm.png (14.01 KiB) Viewed 1372 times
20160304b-worm.png
20160304b-worm.png (31.82 KiB) Viewed 1372 times
20160304b-worm.FCStd
(443.25 KiB) Downloaded 19 times
If you have any questions, post back...

OS: Ubuntu 14.04.4 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6532 (Git)
Build type: None
Branch: master
Hash: 1ec066553e3b018748e75e83e46e7e347c9054ed
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
un1corn
Posts: 155
Joined: Sat Dec 26, 2015 2:06 pm

Re: Chamfering difficulties

Postby un1corn » Sat Mar 05, 2016 3:31 pm

Hello Again.
Thank you to those who took the time to read and responded to my chamfering problem post.

Tanderson69, Sorry I omitted to recheck the geometry on this occasion after including the sketch overlap, once the overlap was removed the errors were also removed.

Mario52, Sorry I was unable get your suggestion to work.

Bejant, I would not of thought to rotate the cylinder to cure the fusion problem nor did I think to use the Boolean cut operation, Both of your suggestions has cured my difficulties and I now have exactly what I want, thank you.

On another note can anyone tell me if the DependancyGraph facility will be available again as each time I have tried to access http://graphviz.org the web page has been unavailable?
Thanks again people.
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sgrogan
Posts: 5800
Joined: Wed Oct 22, 2014 5:02 pm

Re: Chamfering difficulties

Postby sgrogan » Sat Mar 05, 2016 3:53 pm

un1corn wrote:On another note can anyone tell me if the DependancyGraph facility will be available again as each time I have tried to access http://graphviz.org the web page has been unavailable?
Hopefully this is only temporary. I just tried from the US and got timed out.
https://github.com/ellson/graphviz/issues/77
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bejant
Posts: 6076
Joined: Thu Jul 11, 2013 3:06 pm

Re: Chamfering difficulties

Postby bejant » Sat Mar 05, 2016 4:17 pm

The graphviz homepage and downloads page worked for me just now.
http://graphviz.org/Download.php
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bejant
Posts: 6076
Joined: Thu Jul 11, 2013 3:06 pm

Re: Chamfering difficulties

Postby bejant » Sat Mar 05, 2016 4:24 pm

un1corn wrote:Bejant, I would not of thought to rotate the cylinder to cure the fusion problem nor did I think to use the Boolean cut operation
It's handy to remember that when the seams align, that can cause problems.

As for the Booleans, first I used the Part Design WB and had Sketches Mapped onto the planar end faces of your threads. I tried to do two Part Design WB > Groove operations, one on the bottom and another on the top. The bottom one worked (I did that one first) but the top Groove didn't pass Check Geometry, so that's why I used the Part WB > Boolean Difference to make Cuts.
un1corn wrote:Both of your suggestions has cured my difficulties and I now have exactly what I want, thank you.

You're quite welcome.
mario52
Posts: 2921
Joined: Wed May 16, 2012 2:13 pm

Re: Chamfering difficulties

Postby mario52 » Sun Mar 06, 2016 12:07 am

hi
here the graphviz version 2.38 for Windows http://graphviz.org/Download_windows.php

mario
Maybe you need a special feature, go into Macros_recipes and Code_snippets, Dialog creation. My macros on Gist.github.
hiddenengine
Posts: 3
Joined: Mon Sep 05, 2016 3:29 pm

Re: Chamfering difficulties

Postby hiddenengine » Tue Nov 22, 2016 9:16 pm

@Bejant - thank you for the suggestion about rotating. I had the same problem (FreeCAD 0.16.6703) when I tried to chamfer the end of a screw (created with the awesome Fasteners extension). I created a cylinder around the thread, chamfered the end then performed an intersection with the thread. This failed with very spectacular weirdness... until I rotated the cylinder by 10 degrees.

Now it works perfectly.

Does anyone know why you get problems if the seams line up and does anyone know if this will be fixed in a future release? It's good to have a workaround but it would be better if the problem didn't exist... if you have large and complicated models, I suspect that it would be quite tricky to track down if you had a seam alignment causing the problem.