Inventor Drawing Dimension Type

When you are working with some parts you will occasionally have one that, because it was derived or created from a surface, will not be aligned to any of the part origin planes.  The part below is an example of what I mean.

I actually had to work at it to create a part with this condition.  I hope this is a rare occurrence because it can be a real pain when it comes to doing a dimensional drawing.  The first thing you will face is getting an orthographic view looking directly at the part face.  The main reason for writing this article is to tell you about "True" and "Projected" dimensions but since I have to do it anyway, I will mention the process of creating a usable orthographic view.

When you place your base view in your drawing your first thought may be "What do I do now?"  Move your cursor close to the view cube and look of the small icon indicated by the red arrow.  Left click on it to display the view context menu.

From the context menu select "Custom View Orientation".

The Custom View tab will be displayed which contains all your Inventor model view orientation tools and a few more which you can use to square up your orthographic model view.  I will not go into all these tools but two of them are so useful I will mention them.  The "Look At" command will allow you to select any face of the model and square it up to your view.  The "Rotate at Angle" command will allow you to rotate the view to another angle since the View Cube is useless at this point.  Using these tools, I have oriented my model to the desired drawing orthographic view.  To return to the drawing and place this view, select the "Finish Custom View" command.

I now have my drawing view and I have placed my slot center lines and I am ready to start placing dimensions.  This brings me to the main reason I am writing this article.  

When you try to place a dimension from the top edge of the part to the top slot center line, you may have a problem, you cannot place the dimension.  The dimension will be placed on the part width every time.  If you dimension from the top edge to the top arc it will work correctly but you want the extension line gap to the center line.  The problem originated with the part orientation to the part origin.  The solution to this problem is to escape out of the dimension command, place your cursor over the drawing view and right click.  On the context menu, look for the "General Dimension Type" and change it from "True" to "Projected".

You can now continue with your dimensions without issue.  You may want to set it back to "True" when you are finished unless you have other "special" dimensions to place.