Pattern holes within a boundary sketch

[Anonymous]

Hi all,

I'm trying to create a pattern of holes on a plate that will house tubing. The pattern is not that straight forward though. The holes must avoid sections for support steelwork, and the holes themselves must not escape a set boundary constraint. To make the problem a little more complicated, the part is parametric, so if the diameter of the plate changes, or the boundary changes, the hole pattern must increase to fill the extra space, without cutting through the boundaries. To illustrate my part, i have attached a part that was drawn in PRO-E.

The steps are simple in PRO-E; Create the sketches, specify the boundary of the pattern, and fill that boundary with the holes. I have tried using the 'Grill' feature, as that allows boundaries, but not success.

Any ideas? I would like to prove that Inventor can do this, as decisions have just been made to use Inventor over Pro-E, which I fully support.

Kind Regards,
Ryan

[Anonymous]

Hi Ryan,

Believe it or not I have asked the same very
question less then two weeks ago. The topic was "Grill". So far - no
solution to the problem.

Best of luck,

Igor.

--
Web:
href="http://www.meqc.com.au">www.meqc.com.au
        
www.boatworks.meqc.com.au

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

<RyanBotha> wrote in message
href="news:6316594@discussion.autodesk.com">news:6316594@discussion.autodesk.com...

Hi
all,

I'm trying to create a pattern of holes on a plate that will house
tubing. The pattern is not that straight forward though. The holes must avoid
sections for support steelwork, and the holes themselves must not escape a set
boundary constraint. To make the problem a little more complicated, the part
is parametric, so if the diameter of the plate changes, or the boundary
changes, the hole pattern must increase to fill the extra space, without
cutting through the boundaries. To illustrate my part, i have attached a part
that was drawn in PRO-E.

The steps are simple in PRO-E; Create the
sketches, specify the boundary of the pattern, and fill that boundary with the
holes. I have tried using the 'Grill' feature, as that allows boundaries, but
not success.

Any ideas? I would like to prove that Inventor can do
this, as decisions have just been made to use Inventor over Pro-E, which I
fully support.

Kind Regards,
Ryan

[Anonymous]

So I've found a neat little way to create a pattern within a constrained area, using the multi-solid feature. Just create the entire solid, and then split the solid with a sketch. Then create the normal rectangular pattern, but choose the inner solid shape as the affected solid.
You will still have to go afterwards and suppress the holes to lie over the boundary, but thats still better than editing the extrusion of a sketch, or not making it at all.

[Anonymous]

And guess what will happen if you change the
dimensions of your model...

--
Web:
href="http://www.meqc.com.au">www.meqc.com.au
        
www.boatworks.meqc.com.au

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

<RyanBotha> wrote in message
href="news:6318007@discussion.autodesk.com">news:6318007@discussion.autodesk.com...

So
I've found a neat little way to create a pattern within a constrained area,
using the multi-solid feature. Just create the entire solid, and then split
the solid with a sketch. Then create the normal rectangular pattern, but
choose the inner solid shape as the affected solid.
You will still have to
go afterwards and suppress the holes to lie over the boundary, but thats still
better than editing the extrusion of a sketch, or not making it at
all.

[Anonymous]

Hi Ryan,

one of the things I love about Inventor is that almost nothing is impossible, there might be a bit of work involved to do this.

from what I can see you only have two boundaries, the centre hole and the outer border.
If both boundaries are parametrical, you can make your pattern parametrical accordingly.

Make a Parameter, call it X for example. X is the remaining dimension between the outer Diameter and the Inner Hole Diameter.
X = ( Border Diameter - Inner Diameter ) / 2

Make another Parameter, call it Y for example. Y is the number of Holes you can pattern between the X Dimension.
If X = 50 for example and the Holes to pattern have a Diameter of 2 and a distance of 1 between them, you would be able to fit 17 Holes on that X Dimension.
You have to enter the below formula as a VBA function under Tools / Macro / VBA editor, and then bring it back in to your parameters. Let me know if you're having trouble with this and I explain it further.
The below formula will calculate exactly how many holes you can pattern within the X Dimension.
Y = Int ( X - ( Int X / 3 ) * 3 ) / 2 + Int X / 3
Int rounds down to the nearest one.
3 is for Hole Diameter 2mm + Space 1mm.
For X = 50, the above formula should get you 17.

When bringing this back in as a parameter don't forget that this is a unitless number, not mm.
Now you can use this parameter when for the pattern.

The above formula will only calculate the hole pattern for 1 line of holes, just to give you an idea of how you can manage this, you can modify this formula for each line of holes seperately, the next line for example could pattern the holes by the Y value - 1 Hole etc.

I hope this is clear enough.
If not let me know and I can send you an example, I work with features like that all the time and the more complicated they get the more of a challenge.

Regards
Andi

[Anonymous]

You have to enter the below formula as a VBA
function under Tools / Macro / VBA editor...

Huh? WHY?

Брайян Р.
Ивашкевич

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">inventor
specialist

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">
title="http://www.corefurnace.com/ CTRL + Click to follow link"
href="http://www.corefurnace.com/"...

[Anonymous]

I don't think you can enter the "Int" function into the Inventor Parameters. The Int will round down to the nearest one.
I always go to VBA Functions when I have complicated formulas like that and then bring them back into my parameters.
I will write you out the formula as a VBA function and show you how to bring it back into inventor, give me a couple of minutes.

Andi

[Anonymous]

Hi again,

I have attached a word document going through the exact steps I took to achieve the Pattern parametrically.

If done that way you should be able to change any of your Parameters and the Pattern should change accordingly.

Please give me some feedback on this. I'd like to know if it worked for you.

Andi 😉

[Anonymous]

Here's another approach that may work also. I used this same file to
create both shapes. No programming involved.
--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
Instructor/Author/Sr. App Engr. Tel. (260) 399-6615
http://teknigroup.com