Making the 2nd plate match the hole locations of the 1st plate

Matt Smith wrote in news:1190312499.069976.75020 @q5g2000prf.googlegroups.com:

Have you looked into using a hole series? Recent versions can create a series based on an existing hole.

Thanks for the tip. It appears the hole series feature requires that all the holes are done at once through all parts. In my case, I've already done the holes in one part and would like to relate holes in another to them. Doesn't look like it's possible as far as I can tell which is surprising seeing how common the situation is.

-Matt

Matt,

You can edit the second plate in the assembly, add the holes either by sketching them or hole wizard. If you use the hole wizard you can simply create a coincident mate between the sketch points of the new ones and the sketch points on the first plate. I would also advise looking into the functionality of the hole series feature.

Jeff

Jeff,

Thanks for the comment. Your suggested method is how I do it now. The obvious drawbacks are that it takes time if there are a lot of holes and if I change the number of holes in the 1st plate, it doesn't change in the 2nd resulting in dangling dimensions or missing holes.

It appears the hole series feature is the solution. You just have to remember to do this in the assembly from the beginning. There doesn't appear to be an easy solution for when the hole wizard has already been used on a part and you want to copy the locations of those holes to another part parametrically (allowing for adding and removing holes)

-Matt

Matt,

No need for assemblies. It is fairly easy to match features in one part with features in a second using insert part. Here is the trick. In the part that has the pre-existing holes in it create an axis on each hole centerline. Alternatively using surface tools use delete face to create a surface that looks like your solid part. Do this in a configuration. Now, insert that part into the part in which you wish to match the holes. Use the "mates" to position the inserted part and pick the config with the hollow surface in it. You can not match the holes in your new part quite easily. If you change the first part the second will change unless you lock external references.

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P.S. This part can also be inserted into an assembly as an envelope to locate other things without appearing in the BOM.

Too bad. This is the same limitation that usually stops me from using a hole series.

Paul, Thanks for the inspiration. I am working on a product that was started by another design group with a 'master model' technique, and they used Split Part to make the sub-parts (bad idea, at least through all released versions of SWx - we'll have to see about 08). Fortunately, the parting lines are simple, but I was struggling to think about how to handle the mounting bosses. I love your suggestion of using insert-part to bring in the axes of those mounting bosses - I did not consider doing that becasue I don't make too many axes in my biz. Of course, when you insert-part you have the option to bring in axes along with planes (and other items) This could be clean and efficient, more so than in-context references via an assembly in my aplication To add to your post, I would suggest that instead of deleting a face on a configruation of the source part (if I read your post correctly) that one simply delete the solid body of the inserted part as the first (or so) feature of the new part. What I tend to do is insert a part, capture all critical relations in sketches and planes with references to the inserted body, then delete the body so it doesn't interfere with my new work. This (I think) saves the step of creating and managing a new config of the parent part. But thanks for posting - I think your suggestion of axes has saved me some time and head-scratching Ed

Just a clarification (I think) for those that don't normally do this kind of thing. Deleting the body as Ed described is a feature, not actually kicking it out of there never to be seen again, like deleting a part in an assy. That way it doesn't interfere, doesn't add to mass properties, but the info is still accessible if needed.

WT

Well the jury is out on just what to make of the solid on the imported part.

1. Leave it as a solid. Will serve as an envelope in an assembly Can be deleted (not the import, the solid) after importing Usefull for mating and positioning Parametrically tied to original part

Down side is that it can accidentally not be deleted and then count as a extraneous mass. Can add lots of extra faces to render/clutter

1. Remove one face and create a hollow "box" of reference surfaces. Will do all that (1) will do without the down side

1. Just bring in planes, axes and other reference geometry. Super lightweight. Won't slow down or clutter screen.

Down side is that you might lose your sense of direction on which axis does what.

I started looking at this kind of stuff like the old drilling jigs and fixtures. I would make a part with just a few reference surfaces/ planes/axes in it that everything had to fit up to. Then I could use it in parts and assemblies to maintain fit up in the very robust manner and still keep parametrics alive.

It isn't exactly my idea, there was a presentation at SWW two years ago that used this for ship layout.

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