Assembly Feature Hole now how to get info into part drawings

I used Assembly Feature Hole to make some bolt patterns that pass thru
multiple parts in an assembly. Lets say a plate thru a gasket to another
plate. Added fasteners the whole nine. Now I want the gasket part and
subsequently the gasket drawing to reflect the holes I added in the
assembly. How without manually inserting new holes on the part level do I
get the hole information to the part level, but this defeats the purpose of
adding holes in the assembly?

 

This is true. However, the actual manufacturing process probably won't
produce the holes that way either, as evidenced by the fact that you want
the holes to show up in a piece-part drawing. The better way to do it
top-down would be to put holes in the top plate (or whatever you choose) and
then edit each of the other 2 parts in the context of the assy, converting
the holes so they follow. That way, as long as SW can find the "master
hole" part, the other parts will show the correct holes in their own
drawings.

WT

 

In your assembly, make a configuration called, "Gasket only," "plate only."
Then you hide or suppress all other parts (I usually hide instead of
suppressing them to maintain the mates, but this will not report the correct
weight/mass if you hide because it includes the weight of hidden components.
If you don't use the weight of your part in the drawing, then this will not
be a problem.)

Create your drawing with the assembly config, "gasket only".

In my assembly template, there is a configuration specific "part name",
"material" etc, so when the assy is dropped into the drawings, they all
automatically fill out the title blocks. Before you dimension the drawing,
you can "save as" gasket.slddrw", "plate.slddrw", etc, each drawing, then go
back in and change the properties to each individual "Gasket only", "plate
only" assembly config.

I hope this helps,

Dan B.

 

The correct way to do what you are after is by using the hole wizard &
selecting the 'Hole Series' tab, then follow the bouncing ball!!

Merry

 

Hi Merry,

I forgot about that, you are correct! That creates a hole in the assembly
AND the holes in the individual parts. My method works for other than the
holes....

Dan B.

 

You have 2 choices. If you need the hole drilled in the assembly -
like in a sheetmetal angled part - keep the references to the assembly
and make an assembly feature. But if these are machined parts, after
you create the assembly feature hole, return to the part and break the
references. You will have 2 areas to check, one is in the sketch and
the other is the sketch plane. The you can use these parts in any
assembly and the holes will be in the right location and controlled
individually. Regards, Marie

 

Thanks all for the advice and suggestions. I know the "proper" way to do
it, but I backed my self into a corner. I was looking for an easy fix for
the specific predicament I got myself into. After calling my reseller's
"help" line they told me I was done and had to redo the parts. I asked
could I copy and paste the hole feature to individual parts. They told me
no. I tried anyway. Guess what? It worked. It took a little realignment
with the origins, but it was easier that recreating the parts. Hole series
is the way I will do this in the future.