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can INV dimension the slot which was generated embossing on a cylindrical body

18 REPLIES 18
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Message 1 of 19
dho
Enthusiast
1574 Views, 18 Replies

can INV dimension the slot which was generated embossing on a cylindrical body

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.

 

 

18 REPLIES 18
Message 2 of 19
bob_holland
in reply to: dho

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?

 

 


Bob Holland
Autodesk Product Support
Message 3 of 19
dho
Enthusiast
in reply to: bob_holland

that would be a way. but i just wonder if INV will do that AUTOMATICALLY
like it puts up all the views.
(i did not dimension it, i was just exploring the capability of the INV.)
thanks.
Message 4 of 19
dho
Enthusiast
in reply to: bob_holland

second thought. the export - import will lost the LINK.

agree?

Message 5 of 19
johnsonshiue
in reply to: dho

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!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 6 of 19
dho
Enthusiast
in reply to: johnsonshiue

since the feature is "wrapped" around a cylindrical body, your way seems not working. would you try it, if it works?

thanks.

Message 7 of 19
mrattray
in reply to: dho

I can't look at your part file because I'm still on 2013. Speaking of which, it would be helpful if you would mention your version in the post so we don't have to find out the hard way.
Can you post an image of the part, I have a feeling that you can accomplish what you're after using sheet metal tools.
Mike (not Matt) Rattray

Message 8 of 19
dho
Enthusiast
in reply to: mrattray

sorry, INV2014.

here is a screen shot with the sketch shown.

thanks.

 

slot.jpg

Message 9 of 19
WHolzwarth
in reply to: dho

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

EESignature

Message 10 of 19
bob_holland
in reply to: WHolzwarth

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.


Bob Holland
Autodesk Product Support
Message 11 of 19
dho
Enthusiast
in reply to: bob_holland

when set the solid to invisible, the dimensions disappear. right or wrong?

thanks.

Message 12 of 19
WHolzwarth
in reply to: bob_holland

Hmm, Bob. How could you share the emboss sketch?

I didn't see this option in my files. See attached.

 

Walter

Walter Holzwarth

EESignature

Message 13 of 19
bob_holland
in reply to: WHolzwarth

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?


Bob Holland
Autodesk Product Support
Message 14 of 19
WHolzwarth
in reply to: bob_holland

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

EESignature

Message 15 of 19
bob_holland
in reply to: WHolzwarth

Walter,

 

Here you go.

I think that the only part you were missing is Get Model Sketchs.

 

 


Bob Holland
Autodesk Product Support
Message 16 of 19
WHolzwarth
in reply to: bob_holland

Thanks, Bob. That did it.

Smiley Embarassed I tried to do that with clicking at the feature (no success), instead at the part icon.

Walter Holzwarth

EESignature

Message 17 of 19
dho
Enthusiast
in reply to: bob_holland

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?

Message 18 of 19
bob_holland
in reply to: dho

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.


Bob Holland
Autodesk Product Support
Message 19 of 19
dho
Enthusiast
in reply to: bob_holland

dim.jpg

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