Hello
I'd like to make a series of sldprt in order to represent the various machining steps (without going through configs).
So, I create my first piece and I insert it into the second without breaking the links.
But if I fill in the material in my first piece, it doesn't follow in the others.
Is there a solution?
Thank you in advance.
Julien G.
Maybe by filling in the first material and then doing "Copy As" to create the next ones.
Thank you for your answer Alain but I would like to keep the links between the different pieces so that if I modify a hole on the first one, it also changes on the following ones.
It doesn't seem to me that it's possible to create pieces that are linked together in this way.
On the other hand, why don't you want to use the configurations? Especially in your case, it seems like a good idea to me.
Hello
I don't think there's a stock SW solution to do what you want. The configs solution seems to be the safest. Otherwise a macro development could work, but you have to master the subject at a minimum, I'll leave that to the experts (especially @.PL).
However, I will see a trick... Or even a hack. This would allow you to recover the geometry and the material property. I say the property, but not the material as such.
My idea is to use SW's symmetry function. Take your original part, click on the plane of Face (for example) and then Insert/Symmetrical Part. A new room opens up and you're given options. Choose "Template properties" (I'm doing it from memory, it may not be the right text, it's towards the end of the list) and confirm. This way you get the symmetrical of your part in symmetry :/ but above all its material property!
Then make a symmetry of this body without merging. And finally right-click on the original body (the one in the wrong direction) and click on "Delete body".
It's a long time to describe but it fits in 3 SW functions on your child piece. And you have your property matter of informed.
@Benoit: In fact, you make a symmetry function of a symmetrical part;)
That's it, and as 2 plane symmetries cancel each other out, we land on our feet! :)
Thank you all.
Indeed, with "symmetrical part" the material properties remain!
To answer your questions, it is true that going through the configs would be simpler but we want to be able to generate DXFs of each step and be able to evolve one step in EPDM without impacting the others.
Ah EPDM.... It depends on what you're doing as a modification via the workflow. A change of state? If so, the configs are not suitable.
Otherwise, another idea, insert your part into an assembly, rather than into a part. You could recover the material by annotation very easily (less easily, if at all in the cartridge, or the annotation placed on the cartridge!). It involves only material removal operations (or passing through virtual parts in the assembly).
It is indeed changes of state that I would like to make.
It seems to me that in an old version, a FROM PARENT appeared in the material.
Good idea for the assembly but unfortunately I couldn't drill with SolidWatch (I know, I accumulate...)
Yes, you accumulate... :)
For me, the FROM PARENT is at the level of the properties of the document (as proposed with symmetry), not directly on the material of the part.
HS: What does SolidWatch bring you?
SolidWatch allows us to be able to carry out tapping according to watchmaking standards (for example: S0.50), to set tolerances in μm, watchmaking cuts, special mouldings or bevellings, etc.
Why -1 @.PL ?
Thinking about it, with EPDM, the proposed solution might not be compatible :/
Check the settings of the data card assigned to this type of part. Look at what is recovered for the material. Is it a property of the document or directly the SolidWorks material? I have a doubt, it's been a while since I set up an EPDM card :/
In addition, I have tested, during a part symmetry, the material is applied to the new part (identical to the original), but does not seem to follow if the material of the parent part is changed. Except that the property linked to the parent is updating well. As a result, we can end up with a SW material that is different from its property which appears in the drawing :/
My hacking solution doesn't seem any worse than it originally looked. It's up to you to judge.
@Benoit Thank you very much for the tests and the time dedicated!
I'm going to test all that!