Strange boolean operation

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!
jmaustpc
Posts: 9639
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Strange boolean operation

Postby jmaustpc » Wed Dec 28, 2011 2:26 pm

Hi Fred

Try experimenting with all the different tools in the different workbenches, being beta code, often things don't work completely or as you may expect but in FreeCAD there is almost always some alternative method available. Even if sometimes, like I had to today, you have to go to the command line to get what you want, because FreeCAD can do it but the limitation is in the gui passing the command to FreeCAD.


Anyway go to Draft and try Yorik's really cool "array tool" and then you might find that under some circumstances you can use his "draft to sketch converter" and get around your problem that way (or may be not?).

Also for bolt holes, as Norm I think it was said, you can create the outside and the closed profile circle to create the sketch and then PAD that, it will produce the initial pad without padding the area represented by the inside of the closed wirer/profile (circles or whatever).

Jim
User avatar
angow
Posts: 72
Joined: Sun Dec 11, 2011 2:29 pm

Re: Strange boolean operation

Postby angow » Wed Dec 28, 2011 2:39 pm

Image

Hi Normand,
Everything now works as you described.

I “cleaned” the history and minimized the actions. Additionally I tried to make as much constrains as possible.

1. The hexagons are on one sketch and constrained.
2. The second mount is mirrored and thus constrain to the original.
3. The rod circle is also mirrored and thus constrain to the original.
In this case I chose a pad and the boolean operation. So if I edit just only the radius it changes the mounts and the ground plate at once.

It would be nice if one could constrain the midpoints of the hexagons to the screw holes.

Fred
angow wrote:I noticed that it seems to be impossible to create more than one pocket on a sketch.
Sorry, I meant it is impossible to create more than one pad (circles or whatever) on a sketch (for the rods). But now I know it also could not work in FreeCad if I try to make a boolean operation with more than one part to another part at once.
Attachments
Y_Rod_Mount_2_off_mod.FCStd
(59.17 KiB) Downloaded 23 times
User avatar
NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Strange boolean operation

Postby NormandC » Wed Dec 28, 2011 5:59 pm

Hi Fred,

It's coming along nicely. Your model is not complete though, you have three separate solids (the 2 mounts and the botom plate) that you need to fuse together to have a single solid.
angow wrote:It would be nice if one could constrain the midpoints of the hexagons to the screw holes.
It's coming! That's what we call an external constraint, where you constraint your sketch to existing 3D geometry outside of the sketch. The programming for this feature has already started. :)
angow wrote:
angow wrote:I noticed that it seems to be impossible to create more than one pocket on a sketch.
Sorry, I meant it is impossible to create more than one pad (circles or whatever) on a sketch (for the rods). But now I know it also could not work in FreeCad if I try to make a boolean operation with more than one part to another part at once.
I think I understand what you say. What you're talking about is multibodies. The Part Design workbench Pad feature does not allow it. The idea is that in this workbench, you are working on a single part, and a single part does not have multiple non-touching bodies. So when doing your first Pad in a part, the sketch must only have one closed profile. Once your first feature is done, you can pad multiple closed profiles, provided you sketch is supported by a face.

As for boolean operations, you can work with 2 bodies at the time, but if you want to subtract more than one body from your main body, what you can do is fuse the bodies to subtract first, even if they are not touching, it will work.
User avatar
NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Strange boolean operation

Postby NormandC » Wed Dec 28, 2011 6:11 pm

jmaustpc wrote:Anyway go to Draft and try Yorik's really cool "array tool"
Hi Jim,

Is the polar array tool working for you? The rectangular array works fine, but I get nothing when I try to use the polar settings. If I'm not the only one, I'll report this as a bug.
carlod
Posts: 81
Joined: Mon Oct 03, 2011 2:52 pm

Re: Strange boolean operation

Postby carlod » Thu Dec 29, 2011 9:54 am

Sometimes I use a different approach to design parts like this, removing material instead of building, like a milling machine..

Try my attached file to see a way to create the part usin only the partdesign workbench.
Attachments
TEST3.FCStd
(43.88 KiB) Downloaded 29 times
User avatar
NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Strange boolean operation

Postby NormandC » Thu Dec 29, 2011 5:40 pm

Nicely done carlod! :)

Have you tried the new "Refine shape" command from tanderson69? It's in the Part menu (Part workbench), but you need a 0.13 version (there's no Windows installer available yet)

Before:
Image

After:
Image

One drawback is it's not parametric. So if you change your model, it won't update so you have to delete it and run the command again. This is why I use it only at the end.
wmayer
Site Admin
Posts: 15756
Joined: Thu Feb 19, 2009 10:32 am

Re: Strange boolean operation

Postby wmayer » Thu Dec 29, 2011 6:37 pm

One drawback is it's not parametric. So if you change your model, it won't update so you have to delete it and run the command again. This is why I use it only at the end.
The plan is to add this refinement function into the pad/pocket/boolean operations so that everything is done automatically and parametric. However, before doing that you guys should make heavy use of this function to see if we have any problems somewhere.
carlod
Posts: 81
Joined: Mon Oct 03, 2011 2:52 pm

Re: Strange boolean operation

Postby carlod » Fri Dec 30, 2011 7:43 am

normandc wrote:Nicely done carlod! :)

Have you tried the new "Refine shape" command from tanderson69? It's in the Part menu (Part workbench), but you need a 0.13 version (there's no Windows installer available yet)
Thank you

I know about the new feature, but since I don't build by myself, I'm waiting for the first 0.13 unstable to test it.
User avatar
angow
Posts: 72
Joined: Sun Dec 11, 2011 2:29 pm

Re: Strange boolean operation

Postby angow » Fri Dec 30, 2011 2:20 pm

jmaustpc wrote: Anyway go to Draft and try Yorik's really cool "array tool" and then you might find that under some circumstances you can use his "draft to sketch converter" and get around your problem that way (or may be not?).
I find neither the “array tool” nor the "draft to sketch converter". Is it because I use Windows and FreeCAD_0.12.5284?
Would it be possible to make such a sketch (witch is from draft converted) pararetric?
This would open up many application possibilities like importing dxf and make it parametric.
jmaustpc wrote: Also for bolt holes, as Norm I think it was said, you can create the outside and the closed profile circle to create the sketch and then PAD that, it will produce the initial pad without padding the area represented by the inside of the closed wirer/profile (circles or whatever).
Sorry Jim, that what you try to explain me is to high for my limited knowledge of English. I do not dare to ask to show an excample...;-)
normandc wrote: It's coming along nicely. Your model is not complete though, you have three separate solids (the 2 mounts and the botom plate) that you need to fuse together to have a single solid.
What is the difference between a boolean und a fuse union?
The fuse union want’s to select faces. Is it equal wich face or faces from each part I select?
normandc wrote:So when doing your first Pad in a part, the sketch must only have one closed profile. Once your first feature is done, you can pad multiple closed profiles, provided you sketch is supported by a face.
Sorry Normand, the same as I said to Jim - my poor knowledge of English...and I don’t dare...
normandc wrote: As for boolean operations, you can work with 2 bodies at the time, but if you want to subtract more than one body from your main body, what you can do is fuse the bodies to subtract first, even if they are not touching, it will work.
Thanks, I didn’t expected this. This is not working in AutoCad ;-)
carlod wrote:Sometimes I use a different approach to design parts like this, removing material instead of building, like a milling machine...
Hi carlod
Your complete mill way is very interesting.
Though it produces a lot less eco-friendly waste :D

I don't understand Sketch003. How can you change the radius of the half circle?
Whatever I try to edit it will always become over constrained. Where is it hidden? ;-)

Fred
carlod
Posts: 81
Joined: Mon Oct 03, 2011 2:52 pm

Re: Strange boolean operation

Postby carlod » Fri Dec 30, 2011 2:36 pm

angow wrote: I don't understand Sketch003. How can you change the radius of the half circle?
Whatever I try to edit it will always become over constrained. Where is it hidden? ;-)
the arc radius constrain is behind the vertical "30" constrain.