Modification of assembled parts
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Modification of assembled parts
Hi guys,
links points assigned to my parts will be moved when the shape of a part is changed:
Before (watch the datum point in the middle) :
After inserting pockets into this part the datum points appears in another place (one on the outer side, the other on the lower side)
In this situation the whole assembly crashes. I'd try it in A2Plus and Assembly4 with the same result
Maybe you solve this issue many times but I can't find an answer here
Thanks in advance
Winfried
links points assigned to my parts will be moved when the shape of a part is changed:
Before (watch the datum point in the middle) :
After inserting pockets into this part the datum points appears in another place (one on the outer side, the other on the lower side)
In this situation the whole assembly crashes. I'd try it in A2Plus and Assembly4 with the same result
Maybe you solve this issue many times but I can't find an answer here
Thanks in advance
Winfried
Re: Modification of assembled parts
Welcome to the forums Winfried.
In A2plus there are two update options for modified parts. The first is a yellow and green icon, the second is black and orange. The yellow and green works best if you have modified sizes in the part file, the black and orange works if you have added or subtracted features in the part such as you have. The black and orange only allows you to update one part at a time and if the constraints are missing features at the end of the update, a viewer with a table will show that, hopefully, will give you a chance to attach the missing feature.
The messed-up constraints are caused because the names of the features change when you change a file.
I hope this helps but if it doesn’t and you can attach the files and I’ll be glad to take a look at them.
Dan
Re: Modification of assembled parts
Hi Dan,
thx for the quick response.
In the annex you find my Assy4 files. If you want to I can send my A2 files
Yours
Winfried
thx for the quick response.
In the annex you find my Assy4 files. If you want to I can send my A2 files
Yours
Winfried
Re: Modification of assembled parts
I'm more familiar with A2+ so if you would load those I would appreciate it.
Dan
Dan
Re: Modification of assembled parts
Hi Dan,
here it is.....
To reduce size I compress only the document file. Hope it works.
Winfried
here it is.....
To reduce size I compress only the document file. Hope it works.
Winfried
Re: Modification of assembled parts
Winfried: Looks like you are having problems with constraints pointIdentity_001, pointIdentity_003, pointIdentity_017 in Partc_001. Also, pointidentity043 in Keel1_001. This is a fixed part and may be giving problems because it is fixed. There should be just one fixed part per assembly.
A lot of parts will turn yellow indicating that they are not connected to a fixed part by constraints but once you fix the first three constraints it may straighten out.
Good luck.
Dan
Re: Modification of assembled parts
Hi Dan,
you're right. But I can show you how I come into this situation:
Here is a simple assembly, only two parts connected by a ptp constraint:
Adding a pocket into part2 and recalculation of the assembly:
It seems that the assignment for part2 is changed when adding some lines/ points
Yours
Winfried
you're right. But I can show you how I come into this situation:
Here is a simple assembly, only two parts connected by a ptp constraint:
Adding a pocket into part2 and recalculation of the assembly:
It seems that the assignment for part2 is changed when adding some lines/ points
Yours
Winfried
Re: Modification of assembled parts
See TNP.
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Re: Modification of assembled parts
Hi Chris,
not very promsing! Means that the assemby workbences are useless for design?
Seems I have one option: Roll back to the sketcher and parts workbench and paste parts together with draft workbench
yours
Winfried
not very promsing! Means that the assemby workbences are useless for design?
Seems I have one option: Roll back to the sketcher and parts workbench and paste parts together with draft workbench
yours
Winfried
Re: Modification of assembled parts
No most probably your workflow is not correct and expose you to the TNP problem, the link above from @chrisb explain the problem.
To summarize things:
You should not reference to anything that will change when you modify a solid, as the "solid references" like Face number, edge number, and point number and so on could be modified when the solid is changed.
It is better to refer to some other references, that are more "stable" like datum of master sketches, sadly there is no "Universal solution" as they depend on what you are trying to do.
TNP in future will be "mitigated", so it will be more easy to refer to something that maybe change in "number", like when "face4" became "face7" due to some modification but substantially remain similar, as example if you add an hole so it is not a simple "planar continous face" or maybe add some features, like "fillet angles".
TNP could not be avoided, thing of a case when you model a cube and refer to the upper face and then it became a pyramid, some faces are existent although they have changed order, so "left side" could be "described" both in the cube and in the pyramid, but in this case "top side" in a pyramid is disappeared and is imply the point were the four sides will meet.
Same for assemblies, stability has another sense in this case, but even in this case, if you reference to something that "disappear" it will be difficult to "amend" a conceptual error.
Think as example you make a face with a hole in the middle, to accomodate a "set pin" and obviously you want that the "set pin" that probably is attached to another object will go in that hole.
If you delete the hole what happens?
Some ideas:
- CAD will have to tell you, "you could not delete this "feature" as it is referenced by ...., ...., .... elements", and refuse to delete it.
- Same as above but will permit to delete the "feature" and leave model broken as "You have been warned" so it your duty to "make a stable model".
What do you prefer? I'm almost sure that if you ask 10 users you will have at least 15 answers, (comprising 1, but in some case even 2) or maybe more, hoping not more than 20 but this is not guaranteed as I have not take in account ("I don't care", "it' none your business" or similar answers)
But you have some solutions:
- Ask here but please add infos as requested in: https://forum.freecadweb.org/viewtopic.php?f=3&t=2264 as result and behaviour could depend on some versions of libraries, or the Addon itself. And this procedure will supply "helpers" with almost any data they will need to maybe tell you you are using an outdated version of something, or maybe it is a know problem of xxxx, (read FC version, AddOn version and so on.)
- Try to make maybe a "Minimal Working Example" (MWE for short) that show the problem and ask: "how I can make this... without incurring in problems"
Regards
Carlo D.
Last edited by onekk on Mon Nov 14, 2022 12:56 pm, edited 1 time in total.
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