Is there a way to modify your part template to have your desired c'bore fit in that specific template?
If you mean to have a blank template that contains information about a specific hole size, the answer is no.
But there are a number of ways to tackle this particular desire. The most obvious would be to edit your Hole Wizard; add a custom hole standard and then you can change c-bore dims in that standard to your heart's content. The bonus of this method is that you can access those hole sizes from any part, old or new. The downside is that if your desired hole shape doesn't match the existing standards, you're pretty much SOL.
It's been a while but I don't think the Hole Wizard allows control of tolerances, last I remembered. If you want specific tolerances to carry through the dimensions of the counterbores from part to drawing, I would recommend making a library feature or set of features. Make a custom c-bore, add tolerances to the dimensions in the model, and then save that feature to the design library. Next time you need, just drag-drop and you're all done.
Thanks for the input, the c'bore I want is a std within the hole wizard ( 1/32 clearance) but I have to select the fit I was wanting to see if the hole wizard could be preselected with this specific fit so I wouldn't have to remember every time.
Yeah it sounds like you want to "store" a specific tolerance value for that hole. A Library Feature is a great way to do this and they are very simple to make:
1. Create a new part and create a simple shape of some kind like a square plate.
2. Create your 1/32" clearance c-bore on the plate, just one will do. This is important: Delete all the sketch relationships to the placement point (if you create the point at the origin of the sketch, for instance, you will likely need to delete the "coincident" relationship). The hole end-conditions will carry through, usually for a clearance hole "Up to Next" is a good choice.
3. Once the hole is placed, double-click on some part of the hole geometry to display the hole dimensions.
4. Change the dims and/or tolerances as necessary.
5. Select the hole feature in the feature manager tree.
6. With the feature selected, click on the Design Library tab on the right side of the viewport window and then click the first button "Add to Design Library" (it's the stack of books with a green "+").
7. A little interface will appear in the Property Manager where you can choose where to save the feature and what to name it. Name it something that will be easy to identify later.
8. OK and you're done! If it asks if you want a simplified library feature, I always say no using this method. Hard to get simpler than a plate with a hole in it.
To use: In any part document, drag this sldlfp onto the surface you want the holes. A familiar hole wizard sketch shall appear and you can add as many instances as you need an dimension as appropriate in the context of that part. In the drawing your stored tolerances will carry over if you use the Hole Callout tool, no need to import model dimensions.
Thanks I appreciate the help.
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