Fill Pattern - Instances

[SnTMan]

First off, I'm not too good with SW. I'm on 2011 SP0. Don't ask.

I am using a fill pattern to create a large number of holes in a plate. I am getting the idea that SW has no means to tell me how many holes I've got.

I've searched this site (kind of briefly) and find a reference in the SW Knowledge Base to an API, which I assume is a kind of macro. I get the impression this capability is not built in.

Do I have to print and count the holes?

Regards,

Mike

 

[CorBlimeyLimey]

If you used the Hole Wizard to create the seed hole, using the Hole Callout in a drawing view will show the number of holes.

 

[SnTMan]

CorBlimeyLimey, I would prefer to know as I model, know any other way?

Thanks,

Mike

 

[SnTMan]

On second thought, I guess that's better than printing and counting, and I'll try it, but still...

 

[Updraft]

SnTMan,

CBL's tip is probably the best way, but it is always nice to know what other ways there are to solve a problem. Short of printing and counting as you had mentioned you could drop your part in a drawing and insert a hole table. It will give you a summary of the sizes and quantities of each hole. Read up on it in the Help.

- - -Updraft

 

[Eltron]

If you want to get really weird you can copy the body of the plate before you do the fill pattern, do a Combine Subtract after, and look at the number of bodies left.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[SnTMan]

Eltron, I got nothing against weird, so I made a plate w/ one hole, copied it, did a fill on the first, then Combine / Subtract. It seems whichever I use as the Main Body (either Body Move/Copy1 or Fill Pattern1, to use the FT names) I end up with one body per the Feature Tree.

Am I misunderstanding something about the process?

CBL Hole wizard not working currently, don't ask, I'll try this later.

Updraft, although a little cumbersome, this seems to work, thanks.

I'll continue plugging away....

Thanks

Mike

 

[Eltron]

You need to make sure that you adjust the feature scope in your fill pattern so that it only affects the original body. Then it should work just fine.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[DerrickH]

I just did a quick test of what you're trying to do, and what I found to work best is to...

do your fill pattern command, start a new drawing, and dump in a hole table. It won't give you a qty for the holes in the hole description column, but the tags will be labled A1 through however many holes you have (my plate went to A52).

Hope this helps!


Derrick Hochgesang
Specials Project Engineer

 

[DerrickH]

Just realized that will be very useful to find out the open area of a perforated panel to calculate flow... thanks for asking this question ;-)

Derrick Hochgesang
Specials Project Engineer

 

[SnTMan]

Eltron, pardon my denseness, I'm not following...

However, what does work, although bassackwards, is to:

Extrude a cylinder (negative hole)
Pattern it

Correct number of instances is now reported in Solid Bodies, FT

Extrude the plate
Combine / Subtract, and you have a plate full of holes.

Instance info is gone, but reappers when supressing the combine.

Well, whatever works, works

Thanks to all

Mike

 

[Eltron]

OK. Create your part however you like. Before you do the fill pattern go to Insert/Features/ Move/Copy. Select the part (the body that you need the holes in) and click OK. You should have two identical bodies occupying the same space. Now you can do your Fill Pattern, just be sure to adjust the Feature Scope in the Fill Pattern dialog so that it is for only the first body (uncheck Auto-Select). You should still have two bodies; one with the holes and one without. Do a Combine/Subtract. You have to select the body without the holes as the main body. You should be left with X number of bodies which represents the negative of your holes.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[SnTMan]

Eltron, I didn't understand the copied body ocuppied the same space. Got it now.

This may not turn out to be my procedure of choice, but interesting all the same

Regards,

Mike