I designed a chassis with very particular aluminum profiles for a customer, which led me to review/learn how to insert this profile into my profile library. When creating the . SLDLFP, you have to right-click on the sketch and choose "add to library", so a small "L" software appears on the sketch. By the way, where is this library? Because I think I did "add to library" 2 times and in my list of profiles, I have 2 times the profiles available ...
My second problem concerns the use of the adjusting/extending tool for profiles. Sometimes it works properly and I can adjust the profiles, sometimes I can't. So I select the other side of the profile and sometimes it works fine. If it doesn't work I go to another profile and sometimes it doesn't work. It really seems too random to me and I don't think I have the right method to adjust/extend and also create my mechanically welded chassis with the right groupsets. Do you have any information to share on this subject? With a good method?
With my rather random method mentioned above, I manage to extend and adjust all my profiles, except 2 and I have the following errors (PC). Do you have any idea how to proceed?
If necessary I can share my document, but not sure that it is easy because I use a particular profile.
When do I think? Rarely at lunchtime! :=) What do you mean about miter cutting? I tried to do what you proposed to me but it doesn't work any better... I have the same kind of problem.
On your first 2 images, there are 2 things that surprise me: - for a single member to be adjusted, he proposes 7 bodies to keep/delete; - on the second, it is not clear which side is used to make the adjustment.
Can you give us a screenshot of the section of the profile you are looking to adjust?
I don't have too much time at the moment, but I see 3 bodies one and two on top of each other, hence this problem may be, to be checked in more detail.
@stefbeno , see attached the section of the profile. I don't know if it can help... You can clearly see which profile is adjusted and which is not. On the second screenshot, highlighted in blue, the side that serves as an adjustment.
@A.R: I don't understand your comment. I can't see the 3 bodies on my side. Can you explain?
It seems to come from the ribs on your profile! It can be seen that it does not select the entire surface of the end of the profile but only a part of the rib on the vertical profile and the same rib on the horizontal profile. As a result, it does not know how to adjust all the other parts of the end of the profile. (A bit like when a sketch is not complete, you can't do extrusion.)
You have to be able to select the entire surface of the end and not just a part. To be seen with the specialists "who have the right profile to answer" because I never do "extend" or automatic adjustment.
This is not the first time that I see and hear difficulties to adjust extend via complex profiles in the welded mechanic
A walkthrough may be to create your parts directly via an assembly
by registering said parts independently of the assembly
Via your profile sketch it must be possible to extrude to the surface (even if it means creating a surface encompassing your profiles (to avoid negative angles))
@+ ;-)
We can see on your attached images the wacky cutouts
The cut is not identical (left and right) and which of + is, does not follow the profile ?https://www.lynkoa.com/sites/default/files/questions/answer/25/11/2020/erreur_5.jpg
In the screenshot below, I simply made a square with my 4 profiles and here is the result. It is impossible (without adjusting/prolonging) to have a clean and flat cut. Here is the answer I got from the support, which obviously doesn't solve my problem:
"
We also saw that there was a lot of group in 1 single welded mechanic function so I advise you to break down these welded mechanic fct as well as create less group (1 group can be composed of closed lines or several parallel lines)
As for the adjust/extend them, we have seen together that it is a tool and not a function strictly speaking, indeed you can make your adjustments/extensions directly in the group creation which will lighten the tree."
I finally managed to proceed as I wanted, or almost. I must have spent a lot of time with Visiativ support because the profile section obviously didn't help SolidWorks to work optimally. I had too many functions/groups/use of the adjust/extend tool.
I had to review my design strategy for my mechanically welded chassis. The number of groups/functions and the number of times the adjust/extend function can be used should be reduced as much as possible. After the creation of the 5 legs parallel to each other, it was necessary to create a group of 4 profiles representing a parallelogram, giving access to the "miter cuts" option and the "rough cut". You must then uncheck the "allow protrusions" option to make a straight cut. In addition, you have to delete the group you have just created and split it into 2 groups containing lines that are parallel to each other. This forces SolidWorks to pre-register a raw, protrusion-free adjustment of the 90° angles (that's pretty far-fetched). I find this solution quite unstable and it's better not to have to change the 3D sketch afterwards, in which case, I'm afraid it will change the result of the design.
I also discovered in the adjust/extend function the possibility to choose in manual mode what to keep or ignore. When it says "Ignore" or "keep" if you click on this word, it changes its state (ignore becomes Keep and vice versa).
There are other design options that I haven't explored:
- Put the profile sketch in the middle of the sketch line (rather than in a corner, which is my case);
- Make several 3D sketches;
- Rather than using parallel lines or forming a parallelogram, make a "U": parallelogram that remains open on one side.
The profile is attached for the curious.
Admittedly , it's quite tedious and not at all intuitive, for me it's a limitation of SolidWorks.
I hope that is clear enough, but I can possibly provide additional clarifications.
