CAD Challenge #15 - 0.17 - Practice

Show off your FreeCAD projects here!
User avatar
nemesis
Posts: 176
Joined: Tue Mar 25, 2014 11:24 pm
Location: France, Lyon

CAD Challenge #15 - 0.17 - Practice

Postby nemesis » Sun Feb 19, 2017 8:15 am

Hi,
spending my time learning the Part Design Next 0.17 version, try to design things from Reddit CAD Challenge and for the Challenge N°15 this part, and also from other drawing.
Not very complicated, but with one specificity, the draft angle around the part.

here is what I did, and I was wondering if it was a good practice with 0.17, as far as mirroring a body is not possible (should/would it be possible one day?)
Challenge15_moderate.gif
Challenge15_moderate.gif (593.17 KiB) Viewed 923 times



CAD_Challenge15_moderate.FCStd
(286.18 KiB) Downloaded 13 times
chrisb
Posts: 1658
Joined: Tue Mar 17, 2015 9:14 am

Re: CAD Challenge #15 - 0.17 - Practice

Postby chrisb » Sun Feb 19, 2017 9:56 am

I am a bit short in time so I just share my first observations:
- In Part Design you don't mirror objects, you mirror features, there is an icon for that (the frist blue/yellow)
- You have mixed Part and Part Design, that is not recommended.
- You have a body in a body, which seems a strange result of the mixing (some kind of FreeCAD pregnancy).
- The boolean fuse contains only one object, the body. What did you want to fuse it with?
User avatar
nemesis
Posts: 176
Joined: Tue Mar 25, 2014 11:24 pm
Location: France, Lyon

Re: CAD Challenge #15 - 0.17 - Practice

Postby nemesis » Sun Feb 19, 2017 5:39 pm

the boolean operation is the result of fuse between Body and Body001.

Body001 is the mirror of body, as far as mirroring with Part WB don't fuse in single solid.

so.
when I have Half of my part, I mirror pocket003 to have the opposite (impossible to mirror a draft operation and fillet).
once done I "convert" this mirror into a body to allow boolean operation with my first body.

chrisb wrote:- You have a body in a body, which seems a strange result of the mixing (some kind of FreeCAD pregnancy).

well I always have this with boolean operation in 0.17
boolean operation is just a new operation in the main body , from what I understood.

boolean1.png
boolean1.png (98.25 KiB) Viewed 818 times
User avatar
NormandC
Posts: 12071
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: CAD Challenge #15 - 0.17 - Practice

Postby NormandC » Sun Feb 19, 2017 10:25 pm

chrisb wrote:- You have mixed Part and Part Design, that is not recommended.

Sometimes you don't have a choice. PartDesign is missing a "Mirror body" feature. In some cases like the one here, it can be vastly more efficient than mirroring features after features.

Just like sometimes it's much more efficient to use Draft Array.

chrisb wrote: You have a body in a body, which seems a strange result of the mixing (some kind of FreeCAD pregnancy).

I too find it odd, but that work flow is actually intended.

I think it's unavoidable because of the strict "single contiguous solid" policy of PartDesign, a policy which remains controversial to this day, but was decided by jriegel, the project founder.

chrisb wrote:- The boolean fuse contains only one object, the body.

Because this is the new Boolean feature from the PartDesign workbench. It only works with PartDesign bodies, and its aim is to import another body inside an active body and apply a Boolean operation between both bodies.
chrisb
Posts: 1658
Joined: Tue Mar 17, 2015 9:14 am

Re: CAD Challenge #15 - 0.17 - Practice

Postby chrisb » Mon Feb 20, 2017 2:25 am

Thank you for the clarifications. Until now I have only used Part Design artefacts, i.e. bodies in the Part WB and not vice versa, but I will try it, because I see the advantages.
ickby
Posts: 2422
Joined: Wed Oct 05, 2011 7:36 am

Re: CAD Challenge #15 - 0.17 - Practice

Postby ickby » Mon Feb 20, 2017 6:49 am

The boolean in PartDesign is actually a "compromise feature" in the sense that it may be needed for some kind of modeling, but is not intended to be used regulary. It is indeed somewhat strange. The cone boolean for example could be easily and more elegantly be done with a subtractive cone.
User avatar
nemesis
Posts: 176
Joined: Tue Mar 25, 2014 11:24 pm
Location: France, Lyon

Re: CAD Challenge #15 - 0.17 - Practice

Postby nemesis » Mon Feb 20, 2017 6:31 pm

ickby wrote: The cone boolean for example could be easily and more elegantly be done with a subtractive cone.

Sure, the Cone was just an example for the tree boolean example.

The boolean in PartDesign is actually a "compromise feature" in the sense that it may be needed for some kind of modeling, but is not intended to be used regulary. It is indeed somewhat strange.


Well it looks quite logical to me once you accept the concept that the body who receive the boolean operation is the "master" and the one inside the boolean operation are the "tools". it's like any other feature, instead of using a sketch to pocket something, you use a body to "do" something.
I had in mind that one of the purpose of "body" was to be able to add a complex define feature, for example a parametric clip integrated on a plastic part, and re-use this clip in many design easily.

By Easily I mean, just import it in a new part as a body, position/"Assemble" multiple instance of it on the part (same idea LatticeWB does) and then "Fuse" everybody to have a single solid.
A modification of this original body will be propagated to the whole part.

Am I fully wrong?