Hi @outdoorman After rereading your post, I think I answered your question completely incorrectly. Are you just looking to get a radius/diameter dimensional drawing for the part you want to program by hand? If that is the case, this can absolutely be done.
Here is an example of doing this showing diameters as sketch dimensions.
Here is one where I show radius dimensions in a sketch
You can also do it as a drawing showing the dimensions. Note on the right hand view, I show both radius and diameter dimensions on the same drawing view.
Hi @outdoorman I'll show you both methods in two different replies. Both will assume that your part is drawing concentric to the origin. If your part isn't concentric to the origin, let me know and I'll show you how to make a construction axis and the proper construction plane. In my examples I'll be using the origin planes.
Start a new sketch and choose one of the origin planes that runs through the center of your part.
Once you choose that plane, you will be taken to a view normal or perpendicular to your sketch plane. There will be a sketch palette typically on the right side of your screen. Check the slice option. When you do that, your sketch will look similar to the screen shot below, though potentially a different color may be used.
Now you are going to project the ouline of that body. Go to the create menu and then choose Project/Include --> Intersect.
In the Project Geometry dialog, choose the body option and the select your solid body.
Now you can use the dimension command. When you place a dimension, you will get a warning that you are creating a driven dimension. That is fine for what you want to do because you just want the dimensions of the features.
If you want radius dimension, from the Create menu, select point and then place a point at the midpoint of one of the vertical lines on the end of the part. Then dimension from the point to the feature you want the dimension of.
And that is how you can use a sketch to create the dimensions you want. Next I'll show you how to create a drawing.
The second method will be to create a drawing of your part. To do this, from the workspace switcher choose drawings and then from design.
Next you can choose your options such as sheet size and drawing standard. In my example I've left everything as the default for my unit type.
You will get a drawing document that will launch in your Fusion session. You can choose what view of your part you want and you will see a preview of that view when your mouse is over the drawing canvas.
You can change the size of your view by changing the drawing scale. In my example I used a scale of 2. Then place the view and hit OK.
You can place additional views by using the Projected View command. Start the command and then choose the view you want to make a projected view of.
After you select your view, move your mouse to where you want the projected view to appear and press the checkmark to place the view. You can create many projected views at the same time.
Now you can use the dimension tool to dimension your drawing, just like you would in a sketch. Using the dimension tool will automatically pick the correct dimension type. If you select a line or two point, you will get a linear dimension. If you select a circle, you will get a diameter dimension. If you select an arc, you will get a radius dimension. However, if you select a circle and want a radius dimension, from the dimension dropdown, select the dimension type you want.
