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Calling out Counter bores in Drawings.

AndyHermanson
12-Amethyst

Calling out Counter bores in Drawings.

So I have a question. How do you call out counter bores in your drawings? Is there a automatic way to call them out that i am just not finding?

So we have simple hole counter bores in our sheetmetal parts, we then want to call these out on the drawings. The info should all be there somewhere right?

cbore1.png

But we have to manually create the counter bore callout in the drawing.

cbore2.png

This is a dual dim drawing with metric as primary. Shouldn't Creo be able to recognize this as a counter bore in the drawing (or 3D annotation) and show it as something one might use in the industry? It is one feature after all.

Thanks.


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6 REPLIES 6

There is a note feature tied to each hole you create and a subsequent pattern is also recognized. Problem is that a lot of this happens behind the scene using hole tables and some other internal stuff. I am not even sure it recognized dual dim settings.

So it sees the whole and shows it as 3 different dims. but 2 dims are in one orientation and the cbore depth is in another. The dual dims do actually make it all the way through. My requirement is that they are recognized as a single feature not 3.

Right, and that exists. It is a formated note controlled by the hole tables.

holenote.PNG

But there are so many problems with this implementation for drawings that I find it absolutely useless. Dual dimensions just brings the frustration to an even higher level.

This is where it is in the dialog:

holenote2.PNG

Andy,

I ended up creating my own .hol files for c'bored & tapped holes. It works well for me but if you share native files with others that aren't using the same .hol files, you'll have problems.

In the .hol files, there is a table of hole & c'bore sizes. I changed the contents of columns (drill sizes) that I don't use in my notes to the fractional equivilents. I also changed the callout format to my liking.

Capture.JPG

Now, when I want to add a c'bored hole, I have my own thread types in the pull down menu within the hole feature command...

Capture1.JPG

Matt

The difference i see is that you are using std holes and i am using simple holes. The simple holes dont use these notes as far as i know. We dont have any threading or anything these are just for rivets in sheetmetal to "hide" the rivet head below the surface of the sheet...Of course i could be wrong about the simple holes and lack of note.

You are correct. Simple holes don't use the notes. But that is not to say you cannot create them. In general, it has never been simple. And with dual dimensions, you are best off using the applicable dimensions in a note. I typically add the note to the primary through hole diameter dimension so the arrow moves correctly around the hole. Again, I think fully associative drawings are highly over-rated. My drafting skills came from the board. I know how to follow through on all aspect of a design change on a drawing sheet. I don't rely on mindless updates where I have to trust the system to "finish" what I started. All too often, that means you also overlook other things that have changed for completely unrelated reasons. My "product" is the integrity of the -entire- drawing ...anytime I release it.

Just look at how PTC specifies UNC-2B in the note! End of a paramter in a text string ...this is the fit-n-finish I provide for my clients and PTC should take note of. Everything that PTC adds to simplify our lives seem to complicate it for those who care about correctness or completeness. Managing hole notes is one perfect example of advertising hype that simply doesn't deliver to 50% of the users who still rely on complete and accurate drawings. Worse, it spreads the acceptance of mediocrity in an industry I believe in.

As you can see, I care about my drawings. And it seems you do as well. Resign yourself to the fact that if you want it done right, you will have to do it yourself. Manually "crafting" your hole notes is a time-honored tradition in Pro|E.

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