Hello, I did all my assembly, the basis of which is a mechanically welded chassis.
Everything is finished, EXCEPT: that I have to change the thickness of my hollow profiles...
When I make this modification, it becomes horrible, all my constraints are turned upside down, it no longer recognizes the faces, in short, it's s****.
Is there a trick to counter this? Because now to put everything back I have it for a long time....
Thank you in advance, have a good day.
The only solution would be to change the profile sketch, but it would be wrong for all future uses.
Edit: there is a new feature in 2014 that would allow you to keep your references! See this link
http://www.hawkridgesys.com/blog/solidworks-weldment-profiles-configurable/
Is the profile based on a 3D sketch or in separate parts?
I would go into my profile sketch to change the thickness. it will change everywhere
Yes, it's a 3D sketch...
How was your profile created?
and what kind of meeting point adjustment did you make
If you created your profile via your profile library (SLDLFP)
you just have to change your profile or create another one with its own ref
and see the definition of the meeting points of your profile sketches
@+ ;-))
as it is a 3D sketch by changing the sketch of the profile by editing it as said @bart without changing the format its keeps the references. but it leaves the reference in the original thickness.
Having had this type of problem, a great sage of CAD told me that it was necessary to establish the constraints on the plans and not on the faces. So when you change the structure of the tubes, everything stays in place.
So in your case, you have to retype everything.....
What are your points of encounter on your profile
If you made a 3D sketch for your mechanic
So you take as a ref the points where the axes meet?
a copy of the profile with a copy of the mechanic in screnn
I would allow me to grasp the problem
@+ ;-))
Hello everyone,
The software refers to a surface that has a unique code. If you change the thickness of your profile of your sketch it changes the code of the surface so you will have all your constraints to take over.
On the other hand, if you modify your basic sketches by modifying your dimensions, there is no bp because the resulting surface is the same.
I'll try this:
"Save as" your blend.
"Save as" your welded mechanical part
Edit your sketches
Replace your modified part with the new one and see if it bugs.
But personally I have only that to give you.
Good luck
PM
Hello
The problem is that each element (line, circle,...) of the sketch of your .sldlfp file (lib feat part) with the modified thickness must have the same name as the elements of the original .sldlfp file so as not to lose the references.
Normally, if you open the original .sldlfp file, you make a take-away composition that you rename with the new thickness and then in the sketch of the created file, you modify the dimensions without touching the lines and circles, and there normally it doesn't move.
Have a nice day.
See this link
Very good tutorial for the mechanically welded profile under excel
http://www.leguide3d.com/profiles/blogs/profile-mecano-soude-avec-excel
@+ ;-))
Hello
As @dargaud.anthony says, the entities in the sketch must have the same name. In general, it works well on the old profile libraries because they were made from copy to copy with always the same source, so always the same entity names!
In your case, you should try copying the sldlfp you are using today for your welded build and edit just on the thickness. When you go back to SW to change the section for this new profile, your constraints should follow.
See this mechanic welding tutorial
http://www.lynkoa.com/tutos/3d/solidworks-la-mecano-soudure
@+ ;-))
Haha Benoit, we recognize the kings of the hack (yes well, I do the same thing).
That's the big problem with profile libraries. We don't know how our predecessors did them... and we end up with aberrations like this.
In the future, you may want to consider using configured profiles rather than the old 1-file-per-section libraries. (new in 2014 I think)
@flegendre has made available comprehensive profile libraries in the tutorials. The first one is this one for tubes:
http://www.lynkoa.com/tutos/3d/profils-contructions-soudee-configurables-tubes
At least you will avoid this kind of inconvenience.
@coin37coin, I don't really like the "king of hacking":) I prefer long-term solutions, but when you're up against the wall, sometimes you don't necessarily have to try to get over it, but make a hole in it! ;)
You have to use a profile base that has configurations.
That way, you just have to change the line to get the right thickness.
I attach a link:
http://www.leguide3d.com/profiles/blogs/profile-mecano-soude-avec-excel
Since I set this up, it's been great!
@ Bart the link must be good since you also give it ;-))
It is true that it is for a good practice help for profiles
I add and this is important
Don't forget to create your own personal library
in a personal file outside SW like all the libraries
to keep it via SW mutations.
@+ ;-))
Excuse me Gt, I didn't see that you had given this link.. =)
I made a personal base, it takes a little time but in the end, you win
@ Bart ........................... NO pale ;-))
The good refs you have to give them away and not keep them for yourself
@+ ;-))