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Get welding symbol in 2D drawing

10 REPLIES 10
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Message 1 of 11
lis_wang
2001 Views, 10 Replies

Get welding symbol in 2D drawing

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

10 REPLIES 10
Message 2 of 11
lis_wang
in reply to: lis_wang

Is there anyway to solve my problem?

 

Thanks

Message 3 of 11
jozef.dubaj
in reply to: lis_wang

Hello,

 

would you attach the dataset. What Inventor release do you have in use?

 

Thanks,

Jozef

Message 4 of 11
lis_wang
in reply to: jozef.dubaj

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

Message 5 of 11
jozef.dubaj
in reply to: lis_wang

sent you a PM

 

-Jozef

Message 6 of 11
jozef.dubaj
in reply to: lis_wang

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

Message 7 of 11
lis_wang
in reply to: jozef.dubaj

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 

Message 8 of 11
jozef.dubaj
in reply to: lis_wang

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

Message 9 of 11
lis_wang
in reply to: jozef.dubaj

Is that possible to convert my existing main assembly to weldment? It is troublesome to create weldment assembly again.

 

Thanks

Message 10 of 11
jozef.dubaj
in reply to: lis_wang

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

Message 11 of 11
lis_wang
in reply to: jozef.dubaj

I got it.

 

I just know that weldment cannot have position representative.

 

Thank you very much

 

 

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