We are in the midst of implementing design check to do what you are talking about.
This is a tool that can check the very things you are speaking about.
But I typically create my dimensional design intent in my models and import them into
the drawings. But there is no particular method on starting points. Hard to do that
because of the different kinds of parts. Similar parts are done the same way if they
have similar design intents. Again if you setup the design checker it can go through all of this
to make sure things are done as per whatever standard you setup.
With all of that said we try and follow the guide lines of ASME Y14.5-1999 as much as possible.
If you are familiar with the machining or fabrication methods to be used, go through each step in your mind and check that each feature has sufficient information for the procedure.
I use the a counter clockwise dimensioning path (typically). Starting at the best part I work my way around the drawing CCW. My check is can I make a full circle with the dimensions I have listed. On more complicated parts this needs to be expanded to different views, but you get the idea.
Thank you all for your input, I appreciate it very much.
Scott, I am only running the Standard version so it does not have or cannot use the Design Check you link to.
That is too bad. It might be worth looking into to see if it is worth
I think the Auto Dimension feature will take care of your problem.
Auto Dimension imports into your drawing all of the sketch dimensions you used to define you part.
To use Auto Dimension:
Turn [DimXpert] menu bar on: Left click along the margins of your drawing interface to open [Command Manager]
Select [DimXpert] icon to add the tool bar to your screen.
Create a new part model with fully defined sketches. Select [Auto Dimension] icon from the [DimXpert] tool bar.
Select the three reference planes and OK. You will notice a new tab added to the Design Tree and under the tab you will see a dimension tree with all of your dimensions. You can edit these and rename them as you desire.
Create a new Drawing and insert the desirer model views.
From the pull down menu, select [Insert], [Model Items]
In the Command Window, select [Entire Model] and click OK to display all of your model's sketch dimensions.
You can move dimensions around on your drawing to suit your needs or delete those that you do not want to show.
Refer to the HELP section for more detailed explanation of the process and other options.
This method works well for simple parts but a drawing will become pretty cluttered for complex models. I don't use it myself because it takes longer to delete and move dimensions around than it does for me to start from a clean view.
Hope this helps.