Adding dimensions to an assembly in a dwg file

[vasiqshair]

I made a simple TV stand in inventor, and all I want to do now is to dimension the part. There were some I could dimension like the length and diameter of the main shaft, but there were some I couldn't like the slot and bolt holes. E.g. in the left view, I want to show the diameter of, and the distance between, the bolt holes. Firstly, the cursor wouldn't snap to the center of the circle even though the center snap is checked. So I clicked on the circle but Inventor displays a message saying, "select additional geometry or location for dimension". Same with the slot. Please advise. Drawing attached. 

[inchul.lee]

Hi @vasiqshair ,

How were those holes created? Would you be able to share the model for review? You can also send me a private message.

[mikejones · Accepted solution]

Hi 

The problem you have is simply caused by the fact the holes and slots are not perpendicular to the view orientation. If you check you're assembly model you'll find the tube is rotated slightly off axis to the base plate. Either set the orientation of the tube correctly to the base plate such that the holes and slots are aligned to the vertical faces of the base or if the orientation is actually correct and the offset is part of the design intent then you will need to add in two additional drawing views that are ALIGNED to the axis of the holes and slots.

Mike

[thomas.fitzgerald]

@mikejones is correct.  You will need to generate your view differently to ensure you are "looking" at the view from a normal perspective.  Then you will be able to add the dimensions you desire.  If the holes in the model were created at an offset angle then the view orientation, you will need to create an Auxiliary View.

Thanks,

[vasiqshair]

@inchul.lee 

Drawings attached. 

@mikejones 

The slots and holes are at 90 degrees to each other, and I made them using work planes. So if I understand correctly, I just need to re-orient the part in the assembly file before creating the dwg?

[thomas.fitzgerald]

It depends on the intent.  If the holes are oriented based upon a workplane, is the workplane defined correctly?  If so and the holes are accurate relative to the component, then you may need to adjust the orientation of the components within the assembly.  Remember, you should be fully constraining your sketches as well as applying all the necessary assembly constraints.  This is what adds the accuracy to 3D designs.

[johnsonshiue]

Hi! I think I know what you are trying to do. You are trying to dimension the slot. The slot geometry in the drawing view is actually projected from the 3D model to the view. The cut geometry is actually intersection curve (spline), no longer an arc.

To facilitate dimensioning, you can include the sketch from the part. Go to the drawing and right-click on the part in the browser -> Get Model Sketches. The model sketch will be shown on the drawing view and you can dimension the arc precisely.

Many thanks!