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

The 1st plate has a hole wizard feature with a bunch of arbitrary hole
locations.

I'd like to make a hole wizard feature on the second plate that
matches the holes of the 1st without me having to place a bunch of
points and make them concentric to the axis of the holes on the 1st
plate.

I'd done the above many times thinking there had to be a better way.
Anyone know? (This is all 2D sketching by the way)

 

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.

TOP

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

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

3. 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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