I've tried using the 'dimension' tool but it does not allow me to dimension any drafted round. I can't use 'Show model annotations' as the data was imported from a separate file. Any ideas how I can create a dimension for a drafted round? I've never had this problem in Creo 2.0..
Here's an image showing my attempt to dimension the round (which is drafted by 1.5 degrees in the model) using the 'dimension' tool. No dimension shows up when i click the round.
Are you tying to dimension the radius of that edge? Depending on how the round was created. that edge may not be circular, therefore no radius dim is possible. If the part was drafted then the round applied, that edge is elliptical.
Yes I'm trying to dimension the radius. The feature was created as you said; drafter then rounded. Here is another picture showing the part in the model. I've used the measure tool to dimension the radius in the model.
I agree with Doug. In the view you have shown, the radius isn't true and you won't be able to create a dimension.
1. create a leader note and type in the dimension (bad but it get the job done)
2. create an auxillary view that is true to the radius and you may be able to dimension it (depends on the how exactly the model geometry is done)
3. create a sketch that uses the geometry and you can add or show the dimension too (this may end up being a created driven or driving shown dimension)
A variation of #1 would be to create an analysis feature in the model to capture the radius of the cylinder and then show that parameter in the created note. You indicated this was imported geometry, not native, otherwise I'd say just pull the value from the round feature.
If you so have access to the native part, putting the round ahead of the draft, or built into the sketch, will get you a cone instead of a tilted cylinder and you should be able to dimension the radius.
I don't think I've ever gotten a radius dim of something that wasn't an arc or circle. If it's a true ellipse, I've had it ask if I wanted the X or Y radius before, but otherwise there's no radius to get.
Yeah I guess the main problem is that it's an imported geometry and I can't really change how the part is created. I'll keep in mind your suggestions when I create my own models with similar features. Thanks for the help guys!
What is the best practice, to add the radius before drafting the two perpendicular surfaces or apply the draft and then add the radius?
Is it possible for you to put the radius in your tapered extrude instead of a round feature after the extrude?
You should then have a radius dimension.