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setting view with features turned off

7 REPLIES 7
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Message 1 of 8
safiredesignengineers
596 Views, 7 Replies

setting view with features turned off

Hi Group

 

in inv 2014 part mode i want to switch off features like counter sinks on holes as a view  so that when it is waterjet cut only the inner through hole is visible.

i can do this and export the face ok but i then want to show a view in a dwg file with no counter sinks, when i set a new view and then surees the feature it is suppresses in all views set ?  so how can i create views with certain features turned off in the part mode?

 

i havn't installed 2015 yet so not sure if this is the same in there?

 

regards Adrian

7 REPLIES 7
Message 2 of 8

Hi Safire,

 

you can't with view rep, i suggest using a iPart strategy.

 

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-DD9F389B-4B23-482A-A46E-4CA71101658A

 

Hope that it can help you.

 

 

Admaiora
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Message 3 of 8
Anonymous
in reply to: safiredesignengineers

Assuming you are using hole features for your countersinks, there is no way that I know of to turn off just the countersinks.

Possibly you could take the countersinks off the holes, then use chamfer to add the countersinks.  Then these separate features could be suppressed.

 

Message 4 of 8

Assuming you are talking sheetmetal and that you export the face to dxf for the waterjet, can't you just export the back face?


PDSU 2016
Message 5 of 8

thanks for your replies.

 

the ipart solution is a bit long winded based on what i am already doing.

 

I am actually usig champhres for the c/s and i do supress for exporting but then in drawing i want to show a view of the part with no c/s for cutting and another view with c/s for machining.

 

this part is actually a plate and made as a solid as it has C/S on both sides of the part.

 

i am trying to simplify and reduce operations which is why a view rep would work best if it was possible.

 

regards Adrian

Message 6 of 8

iLogic?

Admaiora
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Message 7 of 8
hfds006
in reply to: admaiora

This is most likely not the answer you are looking for, however we use separate models.

 

We model the part "as waterjet". Then derive that part into another model and add the remaining features.

It may not be the most elegant way of doing it but it does mimick the actual manufacturing steps.

 

 

 

 

Message 8 of 8
SBix26
in reply to: hfds006

As long as it's not a sheet metal part, you could do all this in one part by using multiple solids.  Model it without countersinks, pattern it as a new solid a convenient distance away, and add the countersinks to the patterned part.  Then you can create View Reps for the visibility of the two solids and use those in your drawing.

 

Any changes made above the pattern feature will apply to both solids, any features after the pattern will only affect the solid to which they are applied.

Sam B
Inventor 2012 Certified Professional

Inventor Professional 2014 SP2
Windows 7 Enterprise 64-bit, SP1
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