Part design object single solid only?

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kefir
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Part design object single solid only?

Postby kefir » Tue Feb 26, 2019 11:16 pm

Hey, I'm learning more about FreeCAD, but I also discover that there are some details I'm probably not understanding right. Does a Part Design object always have to be a single solid? If some parts aren't meant to touch, do I have to design multiple parts and assemble them with something like Assembly2?

As an example, I tried recreating a ball bearing based on something I saw online, but I structured the part a bit differently. I sketched a couple of circles in Part Design and extruded them to create a cylinder with a hole. Next I'm trying to groove a circle out of the cylinder, to make room for all the balls. Here's what the result looks like at 350 degrees and 360 degrees grooves. The middle section of my ball bearing disappears when the groove is complete.

Screenshot from 2019-02-26 23-55-19.png
Screenshot from 2019-02-26 23-55-19.png (195 KiB) Viewed 498 times
Screenshot from 2019-02-26 23-55-28.png
Screenshot from 2019-02-26 23-55-28.png (188.62 KiB) Viewed 498 times
Is there anything I can do to avoid the middle part disappearing? Why does the middle part disappear and the outer part stay, is there a rule for what stays and what goes? And finally, to design a ball bearing looking like this, and later with all the balls in the "groove", would I have to recreate this design using for example the Part workbench?
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wandererfan
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Re: Part design object single solid only?

Postby wandererfan » Wed Feb 27, 2019 12:23 am

kefir wrote:
Tue Feb 26, 2019 11:16 pm
Does a Part Design object always have to be a single solid? If some parts aren't meant to touch, do I have to design multiple parts and assemble them with something like Assembly2?
"A single contiguous solid" is the original concept for Part Design. Best to think of it as the "Body Design" workbench.

So for your bearing, you'd design a race, a casing, a ball and then combine them into the finished product. You can combine them using Placement properties (see @ppemawn's work in User Showcase), Assembly2+ or Assembly3.

Assembly2 is no longer being developed and Assembly2+ is a better choice. Assembly3 is "bleeding edge" technology.
kefir wrote:
Tue Feb 26, 2019 11:16 pm
Why does the middle part disappear and the outer part stay, is there a rule for what stays and what goes?
There is no rule for this.
triplus
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Re: Part design object single solid only?

Postby triplus » Wed Feb 27, 2019 1:06 am

kefir wrote:
Tue Feb 26, 2019 11:16 pm
Does a Part Design object always have to be a single solid?
Part feature doesn't have to be but indeed body feature currently has a single solid requirement. Therefore what you could do is to first create a Part feature and add two Body features in it. Inner and outer ring will therefore be created as a separate Body features. PartDesign_ShapeBinder can be used to reference geometry from another Body feature. Useful to get more parametric design, if that is desired. Next step would i guess be to create a Part Sphere, use a Draft Array on it. Drag and drop the result in the Part feature.

Such ball bearing would likely be considered as a Part after, although it's basically an assembly. For placing it in some assembly after, one of the Assembly modules for FreeCAD, that starts to make much sense now.
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NormandC
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Re: Part design object single solid only?

Postby NormandC » Wed Feb 27, 2019 4:13 am

triplus wrote:
Wed Feb 27, 2019 1:06 am
Therefore what you could do is to first create a Part feature and add two Body features in it.
A more correct term for Part and Body would be container rather than feature. A Body container holds features. A Part container can hold anything (even meshes), except for PartDesign features.

feature editing
PartDesign Body
Std Part

triplus wrote:
Wed Feb 27, 2019 1:06 am
Such ball bearing would likely be considered as a Part after, although it's basically an assembly.
Well for all intents and purposes, it's both. For someone who purchases a ball bearing, it's obviously a part. For someone who manufactures it, it's an assembly.
Last edited by NormandC on Wed Feb 27, 2019 4:37 am, edited 1 time in total.
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NormandC
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Re: Part design object single solid only?

Postby NormandC » Wed Feb 27, 2019 4:37 am

wandererfan wrote:
Wed Feb 27, 2019 12:23 am
Best to think of it as the "Body Design" workbench.
I've said nothing until now but I really dislike that term. Calling it "Body Design" oversimplifies the methodology. It's like saying you're doing "hammer design" because you're mostly using a hammer in your work. Body is a term that is widely used in CAD to define a single-contiguous volume, which may be solid or not (so a body may be an enclosed shell or a solid). Just like in OCC the term "shape" is used to define most entities apart from meshes. I bet you that no CAD program has ever used the term "Body Design". PartDesign is not just about making bodies. Body is just a tool you use to build the stuff you want.

If people really get confused with Part wb vs. PartDesign wb, then let's rename the latter "Mechanical Design workbench", but please, not "Body Design".
chrisb
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Re: Part design object single solid only?

Postby chrisb » Wed Feb 27, 2019 6:52 am

PartDesign is FreeCAD's "Feature workbench" from what is done inside. Other workbenches have names reflecting the result, such as Part WB, TechDraw, Path, FEM, ... Following that concept, PartDesign is a "Body workbench".

I see many posts and proposals claiming that learning FreeCAD would become easy if we get tooltips here, better names there, improved error messages guiding the user towars a perfect model, ...
I don't say at all that these improvements should be neglegted. But nothing can make learning parametric 3D modeling easy as using a text editor.
A big help would be the previously discussed setup wizard, which generates different configurations for different user groups.
kefir
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Re: Part design object single solid only?

Postby kefir » Wed Feb 27, 2019 9:09 pm

wandererfan wrote:
Wed Feb 27, 2019 12:23 am
kefir wrote:
Tue Feb 26, 2019 11:16 pm
Why does the middle part disappear and the outer part stay, is there a rule for what stays and what goes?
There is no rule for this.

If a body is split into two distinct shapes by an operation such as my groove, perhaps it would make sense to split these shapes into separate Bodies in the FreeCAD document? There may be great reasons for not doing this, but from the perspective I'm seeing it, that seems to be an accurate representation of what is actually happening.

Edit: And perhaps more accurate than simply removing sections after some difficult to understand priority.
triplus
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Re: Part design object single solid only?

Postby triplus » Thu Feb 28, 2019 12:23 am

NormandC wrote:
Wed Feb 27, 2019 4:13 am
A more correct term for Part and Body would be container rather than feature.
We can use a different name in the future, but ATM they are named Part and Body. Therefore user is inserting Part feature and Body feature. If somebody would ask, what is Part feature i have just created? What does it do and for what purpose it can be used for. Then i would provide more clues, such as it's a container, you can put geometry in and move everything around after. I used to suggest it provides local coordinate system, but now local coordinate system feature was introduced, and therefore likely i won't mention that anymore. As some would likely try to put geometry in a local coordinate system feature ...

P.S. Maybe this new feature should be named coordinate system, and not local coordinate system. But such debates are usually fruitless and i don't invest much effort in them anymore.
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wandererfan
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Re: Part design object single solid only?

Postby wandererfan » Thu Feb 28, 2019 2:05 am

kefir wrote:
Wed Feb 27, 2019 9:09 pm
If a body is split into two distinct shapes by an operation such as my groove, perhaps it would make sense to split these shapes into separate Bodies in the FreeCAD document? There may be great reasons for not doing this, but from the perspective I'm seeing it, that seems to be an accurate representation of what is actually happening.
Sorry, not knowledgeable enough for this one. But I'm not sure you want the program deciding how many Bodies are in your design.
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NormandC
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Re: Part design object single solid only?

Postby NormandC » Thu Feb 28, 2019 2:16 am

triplus wrote:
Thu Feb 28, 2019 12:23 am
We can use a different name in the future, but ATM they are named Part and Body. Therefore user is inserting Part feature and Body feature.
Part and Body are not features, they are containers. This is the old "reference constraint" contradiction all over again.
Last edited by NormandC on Thu Feb 28, 2019 2:59 am, edited 1 time in total.