8 Replies Latest reply on Oct 19, 2013 5:14 AM by Dave Krum

# Can't dimension holes in a drawing

I have a round column with holes. I'm not able to dimension the holes in a drawing. I get this message "The selected entity could not be converted into a line or a circular arc. Is there a way that I can dimension the holes in this column, thank you.

• ###### Re: Can't dimension holes in a drawing

The quick and dirty method I use is to go into the feature tree of the drawing view, and set the driving sketch for the hole to “shown”.  Now try to dimension the drawing, and it should grab the sketch rather than the feature.  Go back and hide the sketch and the dimension should stay.  Not very elegant, but I've always been too lazy to find a proper solution.

• ###### Re: Can't dimension holes in a drawing

You can turn on temporary axes to dimension to the center of the hole.

Or you could position your view that your hole is perpendicular to the screen.

• ###### Re: Can't dimension holes in a drawing

Good morning,

Like Paul says above you need to position your hole so it is perpendicular the screen.  One way to do this is to add a plane that is on an angle from the front/right plane, on the same degree as your hole pattern and the other way is to start on either Front/Right planes with you hole, then you can dimension it.

Thanks,

John

• ###### Re: Can't dimension holes in a drawing

Proper drawing technique would be to section the hole

-another option: aux view

--or orient the drawing view so that one of the holes lines up on center

• ###### Re: Can't dimension holes in a drawing

Diego,

That is because in the view you are trying to dimension in they are ellipses not circles.

Don't go the temporary axis route.  Sorry Paul, but in basic training they strongly

advise against that because they are just that, temporary.  You can end up with dangling

dimensions and then you are back to square one.

I would create a straight on auxiliary view to one of the holes to call out the diameter

then create a section view cutting through all of them looking down at them from the top

to create you bolt hole dimensions.

Or place the dimensions in the model and insert them through insert model items.

• ###### Re: Can't dimension holes in a drawing

Creating extra views would be nice and would be prefered but that's not always practical with complex parts.

Show the hidden edges.

Add a centerline between the side lines of the hole.

Then turn the hidden edges off.

Then dimension to the centerline.

The other problem you might run into with holes on a curved surface is the hole wizard callout will not always work.  Sometimes you can select a bottom edge of the hole and the annotation will be connected.  But most times you have to put the drill note in manually.

• ###### Re: Can't dimension holes in a drawing

The best way to create the view you are looking for is create a flat pattern of the part. "Insert, Sheet Metal, Convert to Sheet Metal", once this is completed, you can put a dimension on any hole. You can do what others have suggested with using planes, however, how many holes do you have? Create a flat pattern and show the distance from each other and size and your done.

• ###### Re: Can't dimension holes in a drawing

Thanks for the suggestion.