I have a weldment assembly. It is a subassembly under a main assembly. In the 2D drawing of this main assembly, I tried to indicate the welding symbols for the subassembly assembly. The "Get Weld Symbol" is grey out.
How can I indicate welding symbol in the 2D drawing?
Thanks
Solved! Go to Solution.
Solved by jozef.dubaj. Go to Solution.
Hello,
would you attach the dataset. What Inventor release do you have in use?
Thanks,
Jozef
Please see the attached drawing. I want to add welding symbol at two places, but it cannot. You can refer to assembly to check where the welding symbols are.
I am using IV 2012. As the file is more than 3M. Can I email you? What is your email address?
Thanks
We got a solution. Please put your main assembly into a weldment assembly. Then use the weldment assembly to create views in the drawing. Once the root assembly is recognized as weldment the "Get Welding Symbols" becomes enabled.
Seems that Inventor looks for weldment in root assembly type only. I think it should do it with subassemblies as well. Thank you for your input. I believe this can be improved in future thus I reported this to the developers.
Thank you for your input.
Greets,
Jozef
The "Convert to weldment" is grey out when I tried to convert the main assembly to weldment. Are you redo the assembly in the weldment environment?
Rds
Simply create a new (blank) weldment assembly (template weldment.iam) and use Place command (P key) to insert the assembly you sent me. Then in new drawing document place desired views of the new assembly.
-Jozef
Is that possible to convert my existing main assembly to weldment? It is troublesome to create weldment assembly again.
Thanks
You don't need to convert anything. Just follow the steps:
1) Launch Inventor
2) Press Ctrl+N (New file)
3) Select Weldment.iam
4) Press P (Assemble tab > Place Component)
5) Find and select "air engine_ECO.iam"
6) Save the new assembly
7) Open/create drawing and place desired views of the new assembly
😎 RMC on the view: Get Model Annotations>Get welding Symbols
It is possible to convert also but you will have to delete
air engine_ECO.iam>Representations>Position: Outlet and Inlet
Then Convert to Weldment becomes available
-Jozef
I got it.
I just know that weldment cannot have position representative.
Thank you very much