Anyone, can help with adding custom weldment to library?
Do you mean a weldment profile sketch (.sldlfp) to be used for the Structural Shape function, or something else?
Yes exactly. New created profile to be used for the Structural Shape function.
1. Open a new part.
2. Select a plane and create your profile sketch. Keep in mind that the origin will be the default insertion point when used in the Structural Shape function.
3. Exit the sketch.
4. Click on the sketch in the tree, and while it's highlighted, go to File > Save as... and select "Lib Feat Part (*.sldlfp)" from the drop down under "Save as type:". It's important that the sketch is highlighted when saving. Select a file name, and save at the location specified at Tools > Options > System Options > File Locations > Weldment Profiles.
Thank you Glen.
It looks simple. Do you know if profile can have configurations?
If is fairly simple, but it has to be done correctly. And yes, starting with SW2014 you can have configurations in the sketches. However, I haven't had the time to get mine set up, so I can't answer any specific questions about that. Someone else could help if needed.
Thank you any way. We are still on 2013. Probably will go straight to 2015.
These might be helpful:
The ABC of Weldment Profiles in SOLIDWORKS
Add more Weldment Profiles
How to create Weldment Profile
Wen I try for the SW Content..
It is showing Unable.
Suggest me for the above..
Could be issue/rights on your machine. Please try again else request your VAR to send you the files.
How to request for VAR.
Send a simple email to your VAR (the company from where you've got the SOLIDWORKS) to send you the files or tell them the issue you're facing while downloading these files.
I have tried..
first we have to register in 3D content Central, RMB on "Solidworks Content" --> share a Model ---> then register Free 3D Content Central
After all this. we can access the things..
Thanks for sharing the info.
The easiest way is to open an existing profile, modify it as you desire, then save it with a new name and the .sldlfp extension. The name you give it will be what is displayed in the size drop down of the structural member dialog. If you don't know where the weldment profiles are, go to options, system options, file locations, weldment profiles, and you will see where they are located. Save your profile in the same directory as the other profiles. Add new folders as required to organize. When you insert a structural member you will see your new folders and profiles in the drop downs.
Many times, I want to add a plate to a weldment. I saved a small rectangle profile and use it every time I want a plate. After adding the feature, I go back and edit the sketch of the profile to the plate size I want. You can simply change its dimensions or your can completely change the shape of the profile, if you need an odd shape.
Retrieving data ...