Inventor 2D drawing gives front, left, ... back views from ipt. will it generate expanded view of a cylindrical body surface to be dimensioned (detailed)?
thanks for help.
Solved! Go to Solution.
Solved by dho. Go to Solution.
David,
I took a look at your part and noticed that you did not dimension your slot.
This Inventor works better when sketches are fully constrained.
You can then export the sketch of your slot and the import it into a sketch in your IDW/DWG.
Is this what you are looking for?
Hi! Have you tried "Retrieve Dimensions" in the view? Depending on the view direction, right-click on the view -> "Retrieve Dimensions" -> select the part or the features -> select the dimensions to retrieve. The model dimensions will appear in the drawing view. Also you can edit these dimensions to make changes back to the part.
Thanks!
since the feature is "wrapped" around a cylindrical body, your way seems not working. would you try it, if it works?
thanks.
Try this:
- Workplane on cylinder outer dia
- Project emboss sketch
- Create small surface
- Switch only this surface visible in a separate IDW view and place dimensions
Walter
Walter Holzwarth
Walter,
Thank you.
I have also included a screen cast of pretty much the same steps.
http://screencast.com/t/LHbcDSjLOR8
Please take a look and let me know.
when set the solid to invisible, the dimensions disappear. right or wrong?
thanks.
Hmm, Bob. How could you share the emboss sketch?
I didn't see this option in my files. See attached.
Walter
Walter Holzwarth
Walter,
Sketch 2 appears to have already been shared.
Once it has been shared it shows above the feature that consumed it.
Does this help?
No real help, Bob. I couldn't get this sketch transferred into the IDW.
😉 Well, you have my IPT. Can you add your IDW solution?
Walter
Walter Holzwarth
Walter,
Here you go.
I think that the only part you were missing is Get Model Sketchs.
Thanks, Bob. That did it.
I tried to do that with clicking at the feature (no success), instead at the part icon.
Walter Holzwarth
when retriving the dimensions from 3D model, it works. but with the whole part view with it, a messy thing. if turn off the part visibility, the dimensions go away with it. it can be done to re-dimension the sketch, but it is no longer associated with the model. right?
David,
If you dimension the sketch in your IDW/DWG rather than retrieve the dimensions, your IDW/DWG dimensions will update when you change the sketch that you retrieved.
This way you can turn off the solid body and only have your sketch and dimensions.
Please try this and let us know.