Convert Drawing View to Sketch

[Anonymous]

Is there a way to convert a linked drawing view of a part into a dumb unlinked sketch?

This is a simple feature in Solid Edge and ProE, but I can't figure it out in Inventor.

In my case, I want to create a 2D schematic (a sketch) on an assembly drawing sheet.

In Solid Edge and ProE, I could create a view of a wire nut, right click it and select "Convert to 2D", or something similar.

The view would then become a dumb unlinked sketch, that I could copy and paste numerous times to create my schematic.

The only way I see to do this in Inventor is to create multiple drawing views of the wire nut.

If the wire nut model changes, my drawing will change.

Also, it would be nice to have the entire schematic in a single sketch feature, so I could copy and paste that to other sheets to make variations.

Thank you for your help!

[mdavis22569]

You can copy any base or projected view via RMB in the view and copy ...

Not sure about the breaking the link part ...

here is a quick example I copied views from Sheet 2 and pasted it 3 times on sheet 4 and 44 and 45 are from Sheet 3 ...

They will update with model changes though

[mdavis22569]

2nd options would be to make a derived part of what you'd like to do this too  and then break the link and create views as needed

[Curtis_Waguespack]

Hi Ed.McCracken,

I recall doing this in the past occasionally, by creating the view on the sheet, then saving a copy of the drawing as an AutoCAD *.dwg file (or *.dxf) and then opening the file in AutoCAD and copying (CTRL + C) the "linework". And then going back to Inventor and creating a Draft View or Sketched Symbol and pasting (CTRL + V).

But when you say "schematic" I wonder if you're talking about a 2D sketch in a part file. In which case you might just want to create that sketch as a Sketched Symbol in the drawing, and then you could copy it from drawing to drawing as needed.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous · Accepted solution]

Thank you for the help. These replies helped me find another workflow that seems to fill my needs.

1. Create a drawing view of the part.

2. Select the drawing view, click Sketch.

3. Click Project Geometry.

4. Wireframe select the whole part. Right Click on geometry, select Delete Constraints.

5. Select all lines, drag them off of the part view they were extracted from (so you don't select the view below it). Select all of the lines, Copy. Exit Sketch.

6. Create a Draft View under the Place Views tab. Give it a name.

7. Paste the lines into your new Draft View. When they are pasted, they are set to Sketch Only, so hit the Sketch Only button under the Format section to make them visible outside of the Draft View.

8. Done.

In my case, the Draft View is the main "schematic" or "wiring diagram" so I will paste all of my projected geometry into it. I can then insert new lines (wires) and text into the Draft View to complete my "schematic". This way, the entire schematic (views, sketches, text) is encapsulated in a single box that I can drag around.

[milan5]

what if view include dimension, and want to make sketch of geometry & dimension.

Regards,

Milan Kantaria