Sketch Question

[dbrblg]

Hi,

I have a sheet metal part with an unconsumed sketch (I believe thats what it's called!!).  How do I get the sketch to show in a drawing?

I have tried right clicking on the view and selecting Get Model Sketches from within the drawing environment but it doesn't work.  I also note that none of the unconsumed sketches from within the part actually show in the tree in the drawing environment; only protrusions, fillets etc show.

I am using Inventor 2010.

Thanks

[japike]

Right click on the part in the drawing browser and select "Get Model Sketches".  Then right click on the sketch in the drawing browser and select "Include".

[dbrblg]

Hi Jeff, 

Thanks for your reply.  

I can select the Get Model Sketches option but there are no sketches showing in the tree for me to include!!

Thanks

[japike]

Can you attached your files?

[dbrblg]

Here we are...

[SBix26]

I don't know what's going on, but if I place the same view by defining a custom orientation looking straight at that top surface, I can then include the two unconsumed sketches.  But that top surface is parallel to the XZ plane, so an ordinary top view should produce the same result...

[japike]

Strange!!

Here's what I've tried:

I opened your files and the sketches were not visible in the drawing browser.

I made views of your part in a new drawing using my template.  The sketches would not show up in the drawing.

I made a new part and inserted it into my drawing.  The sketches showed up in the drawing.  So, here I had both my part and your part in the same drawing.  Sketches worked on mine but not on yours.

I inserted views of my part into your drawing and the sketches showed up in the drawing.  Again, the sketches worked on views of my part, but not on views of your part.

So, I'm starting to think there is something wrong with your part.  Can you make a very simple new part with a sketch in it and see if that will show up in a drawing?

[japike]

Really!!!!!

I can't get the sketches to show up that way.

[SBix26]

I placed a new base view, clicked on the "Change View Orientation Button", then used the View Face tool and selected the surface where the sketches are.  That view will include sketches, but placing a top view will not!

[japike]

AHA!

When I use the View Face tool, it works here as well.  Nice one Sam.

Very strange problem.

[Ktelang]

you can xopy the sketches to flatten view.

I dont know whether that works for you

but see the modified attached files for your reference

I got your 2 sketches to show up on flattened view

[SBix26]

More info about the strangeness of this part: the surface with the unconsumed sketches measures 90.000000016 deg from the YZ plane.  Yet it is created as a contour flange from a sketch with the line constrained horizontal, so I am unable to account for this exceedingly small "error".  Only that particular measurement shows any deviation from the expected orthogonal setup, as far as I can tell.  But apparently that's enough for Inventor to consider that surface as not normal to the view.

[dbrblg]

Hello all,

Firstly thanks for all your help.

I tried creating a simple part with a sketch, as suggested by Jeff.  This shows sketches in the drawing, so that works 

I also tried Sams suggestion using a custom orientation on the top face which also works 

So it does tend to point towards the 160 nano degree error on the angle???  Although I cannot see why you wouldn't be able to see the sketch, just that it would look slightly on the wonk (if you could even notice such an angle!!)

How did you manage to find that out?  I cannot even find a precision that accurate.

[SBix26]

In the measure tool (measure angle, actually), set the precision to All Decimals.

[dbrblg]

Oh, thats interesting.

I looked there and set the precision to All Decimals but I could only get it to report as 90 Deg - there were no decimal places 

I wonder what determines the resolution; hardware perhaps? 

[SBix26]

The only angle measurements that showed that error are the horizontal surfaces to the YZ plane.  No others that I could find showed anything other than 0, 90, etc.  You would expect that if there was a "nano-degree" difference between horizontal and YZ, and 0 between vertical and YZ, that between horizontal and vertical you would also find that small difference, but not in this case.

If anyone from Autodesk is paying attention to this thread, we would greatly appreciate some insight into what is going on with this file.

[Hochenauer]

Thanks for reporting this issue, we have identified the cause and development is working on it. I logged DID 1387255.

Sam B, good job on your angle analysis .

Gerald

Gerald Hochenauer(gerald.hochenauer@autodesk.com)
Inventor Principal Software Engineer

Manufacturing Group
Autodesk, Inc.