Accessing User Parameters from Flat Pattern

[Anonymous]

Hey everyone!

I am have been creating flat patterns and dxfs of sheet metal parts that my company uses and one of the things that I have to do on each part is add the part number and project number on each part in Inventor or Autocad manually. When attempting to access the folded model user parameters from the flat pattern, I noticed that all of the user parameters are gone.

My question is...is there a way to access the folded user parameters in the flat pattern?

Thank you!

Sean

Inventor 2018.2

[johnsonshiue]

Hi Sean,

Certainly, the user parameters in folded mode are carried over as reference parameters in flat pattern mode. Activate the flat pattern and go to Parameters table. You should see the reference parameters.

Many thanks!

[Anonymous]

Johnson,

I am able to see all of my numeric user parameters in the flat pattern but none of the text user parameters.

Thank you,

Sean

[mcgyvr]

---

@Anonymous wrote:

Johnson,

I am able to see all of my numeric user parameters in the flat pattern but none of the text user parameters.

Thank you,

Sean

---

@Anonymous They are no longer listed in the "User Parameters" section but are moved up into the "reference parameters" list..

same screen.. Just look up higher.. 

[Anonymous]

I looked and the only one that transferred over to the flat pattern parameters is the numeric parameter. The text ones do not show up. Please see photos attached.

Thank you,

Sean

kelly.young has embedded your image for clarity:

[mcgyvr]

---

@Anonymous wrote:

I looked and the only one that transferred over to the flat pattern parameters is the numeric parameter. The text ones do not show up. Please see photos attached.

Thank you,

Sean

---

My fault.. I didn't pick up on you mentioning numeric vs text..

You are correct.. Text user parameters do not transfer over..

Where do you mark the part number on the flat? 

Not sure if you know this but..

You can do that now with "geometry text" created in the flat pattern..

Go to flat pattern.. Create sketch.. add your text.. right click on text and select "convert to geometry" and select "ISO" or other font..

Finish sketch..

Export face and it shows up in the dxf..

https://www.youtube.com/watch?v=-4xKV13bWGQ

[johnsonshiue]

Hi Sean,

Text parameter is just a string. You cannot use equation or expression to reference another parameter regardless of folded or flat pattern mode.

Many thanks!

[kelly.young]

Hello @Anonymous the only thing that I could see possibly working to link text is though Insert CAD into a sketch.

I couldn't get it to work, but if you saved your drawing as an Inventor.dwg and then inserted it to call the text from there. I think that causes cyclical issues and probably won't work.

I don't think there is any other option to pull text data in the flattened environment.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[johnsonshiue · Accepted solution]

Hi Guys,

I almost forgot about Copy to Flat Pattern workflow. You could push a 2D sketch on face on the folded body to the face on the flat pattern body. Simply create the text sketch in folded body. Right-click on it -> Copy to Flat Pattern. The sketch will be associatively pushed to the flat pattern body. Would it help?

Many thanks!