10,000 plus pattern/entities speed

[SolidsMaster]

So, I've got a part with a series of holes spaced in pattern that is .10" x .10", and the holes are say .05" in diameter. This pattern fills a circle of 10.75". This yeilds a ton of entities no matter which way you slice it. So far, the fastest performer has been a sketch of one quadrant, with a linear pattern. Then a rotated feature pattern. Rebuild times are horrible with even 3GB of ram. Anyone experience this? I haven't tried it with a feature driven pattern yet, but don't believe it will help. Also have imported from Acad as a giant sketch. It's a cruncher!!

Later,

John

 

[Theophilus]

Back in 1997 I did a microscreen for a razor as a sheet metal part on an old dual 300MHz Windows NT workhorse. I had zillions of holes patterned linearly across the sheetmetal part in a flat state. That took long enough. To rebuild the thing, I would process the bends (after the flat was full of holes) and then go take a long lunch. This process gave me more accurate holes in the radius of the microscreen and looked great.

I learned quickly how to stress out what was then a very robust workstation. To reduce rebuild (and all other time), I got the microscreen to a point of completed design (for the most part), then exported it as a parasolid and brought it back into SW. Much better in making a change or two and using within an assembly since it didn't have to process a whole tree of exessively difficult features. But it still taxed the graphics card (Oxygen at the time).

Your RAM will help, but I would guess your processor is the bottleneck in this case. If you watch your Task Manager graph, I would guess your processor is running all the time through the rebuild. You may want to consider using the export-import trick (while saving your original file) for the every-day use within assemblies, etc. In fact, depending on rebuild time, it may be faster to import your perforated geometry and make future changes directly to the "dumb" solid and to forget about referring to your original. This really depends on your rebuild time and the frequency of editing your hole patterns.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[dsgnr1]

SolidsMaster,
I have (and so has Theophilus) broached this subject before.
It may warrant to outline your perforation and note the pattern on the face of the drawing. (just show the perimeter holes or just a few to define the array)

Theophilus,
Can you save as parasolid and then unfold a sheetmetal part?

dsgnr1

¿)

To get the best from these forums read FAQ731-376 before posting

 

[Theophilus]

dsgnr1, no way. Once you've exported to a "dumb" format, you lose everything feature-related in your tree. You can bring in your surface and solid bodies importing from SolidWorks, but you only retain the bodies themselves--no series of features used to create the part in the first place.

One thing you can do, however, is export as a flat piece and export as the folded piece and bring those back into SolidWorks--but each still remains "dumb" regarding your features list and history.

I'm not sure if you could insert bends into an imported part that otherwise has the proper thickness and geometry to attempt to do so--I haven't tried it but I have a feeling that wouldn't work.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[SBaugh]

You can import a Dumb solid into SW and do an Insert\Bends on the imported body. It will then be a fold, unfold SM part, but it is still a dumb solid and you have lost all the Features that made the part to begin with.

There are many stiplations that must be maintained for the insert/bends to work on imported Bodies, but I have done this several times.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[J-C]

Another option instead of exporting would be to Open a new part and "Insert Part" the perforated part. Once inserted, right click it in the tree and select External References. In that dialogue, "Lock" the reference then update only when you choose to unlock it. May still get the benefit of exporting and reimporting while retaining the ability to update if needed.

Back to the orginal question of speed, I don't think any modeler on the market will perform well with this many holes. Oh, and make sure "Geometry pattern" is unchecked in yuor pattern features, not sure if that will help though.

And one last suggestion if this is only for "looks". Don't cut any holes and put a texture of holes on the face. Works well for appearance on the shaded model if that's what you're after.

Jason

 

[SolidsMaster]

So far I've got it down to 1313 seconds (20 min) for the operation, by using a 100 hole pattern, then pattern that in one quadrant, then a rotated pattern. These type of files is where I always here the 2D faster then 3D arguement, in this case I must agree.

Jason - yes, I do have the Geometry pattern checked, but 10,000 holes is 10,000 holes no matter how you cut it. I like the texture idea though for presentation!

Thanks,

John

 

[J-C]

I mentioned Geo Pattern since it disregards end condition for the holes. May not make a difference though.

@d is certainly faster for this as it doesn't have to calculate the 3d geometry each rebuild. Have you tried a sketch pattern of the holes? Do you have to extrude cut them all?

This type of thing brings all parametric 3d modelers to their knees.


Jason

 

[SolidsMaster]

Yes, they all are needed. But, we got around having it made by manually giving him the pattern to have him program the machining. Yes, tried the sketch pattern of the holes. File size is pretty big considering the complexity of the part is simple, besides the holes.

John

 

[davidinindy]

Just from my experience, (which has only been up to 150 objects patterned) large patterns like that are tough, regardless of which 3D CAD you're using.
I've tried it in Pro/E and SW both, with similar results. I also work with UG & Catia users, and they say the same thing. They all ussually use some type of work-around, which often consits of a few of the features that are patterned, and a note on the detail drawing that specifies how many, spacing, etc...

David

 

[SolidsMaster]

That's what we've been doing for now. Oh well.

John