Slanted fill pattern.

[lkasch]

Dear community.

The company I work for hired a design firm to come up with some new design all our machines should follow. The problem is they came up with a design, we cannot make in a reasonable way in Creo.

The final product should look something like this:

The problem is, there's no option in fill pattern to do a slanted pattern.

The best way we have found to create the pattern is to make an oversized sketch pattern like so:

We then make an extrude, where we project the sketches, that fit within the area we need the pattern like so:

The problem we're facing is, that for every project you make in one feature, the slower the machine works.

It doesn't take long before the machine becomes completely unstable and crashes.

I hope you understand my problem, and that someone has a better way of doing this?

Please just ask if I haven't been clear enough in explaining the problem.

Thank you

Lars Kasch

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[JonathanHodgson]

Just my initial thoughts...

You want these slanted features to be holes, correct?

How about:

• Make a flat surface ('fill') somewhere outside your real part.
• Create an 'oversize' pattern as you've already done, but extrude each parallelogram as a capped surface and merge it with the flat surface created above.
• You should now have one quilt with lots of 'finger's sticking out of it.
• Create a surface defining the outside profile of all the holes, un-capped and extending above and below the quilt created above.
• Can you now merge this with the first quilt so that it still leaves a closed surface? If so, you should finally be able to solidify the quilt to cut the holes.

Good luck!

[lkasch]

Hello Jonathan

Thank for the great idea, sadly I can't get program to merge with a pattern.

I tried deleting the pattern, and that made it possible to do the merge.

I then recreated the pattern and edited the merge, but it was still only the first instance that was merged, and it was not possible to add any of the other instances to the pattern.

I also tried to do a merge with one of the parralellograms that overlaps the edge of the border, here I get an error when trying to merge.

I hope I understood your suggestion right and followed it right, but I cannot get it working. Any other ideas will be greatly appreciated.

[John.Pryal]

Hello. Rather than create the slots, create the ribs, would that be easier? Would that even work? I can see what look like radii in the corners of the slots, so maybe not. It was just a thought.

John

[lkasch]

Hey John.

It's worth a shot, but I can't really find a good way of sketching it, so I can pattern it. You're right there's rounds in the corners further complicating matters.

Thank you for the idea though.

[TomD.inPDX]

That is a lot of overhead on the system. I fully understand your seeking a more efficient method.

I am with John on this. Just use a big cutout and pattern --\-- and fill any remaining voids.

If this is a sheetmetal model, you can do this in the flat. That way you can manage any features that might just fall in the bend region. Often, sheetmetal has issues with this so learn the limitations.

[TomD.inPDX · Accepted solution]

We had a relatively involved discussion about complex pattern generation. The outcome was that Creo overhead in merging solids is excessive.

Feature Failure with Repeating Patterns

For your case, if this is a very common feature, I would almost entertain an import feature.

PTC did say they would think about expanding the fill pattern capabilities. I guess they didn't do this for Creo 3.0 (?). Being able to define the fill pattern geometry is almost obvious as a requirement.

I did find one method you might find useful if this is using sheetmetal:

• Create the hole you want.
• Create the --\-- FILL feature with fillets and all for each cell.
• Pattern the fill feature as before
• Merge all the fill patterns. Maybe a find will select them all quickly (?)
• Extrude a surface to trim away the excess
• Use an offset feature to solidify the grid

This removed 95% of the pattern regeneration overhead.

This again was much more challenging than it should have been. Way to many limitations in sheetmetal to make this intuitive. But I think this will solve your regen issue. How to "center" the pattern and managing master sketches is your second challenge. Finding a way to select all the merged surfaces easily is another challenge.

[lkasch]

Brilliant stuff:)

Thank you very much, this is a lot faster than our previous method of doing it.

I hope others with the same issue will find find your sollution, and then I really hope PTC will add functionallity to the fill-pettern feature.

[psobejko]

Hi Antonius,

I don't think this technique has to be restricted to only sheetmetal models.

You can pattern the --\\-- fill element, then merge them at once (just make sure they don't overlap) and you can use the find tool to select the quilts at once:

After that, you can trim away the outside, then merge the flat grille with the outer part of the panel. Then you can thicken this surface to make a solid... Also note this uses "Geometry Pattern" so it is fast.

[TomD.inPDX]

Of course, you are right, Paul. The technique is actually from solid part modeling. SMT just throws some curves to the solution. I certainly recommend this method for solid forms as well.

We did learn earlier that typically geometry patterns are more efficient, and in the case of the fills, it likely is. But when they are solid, they have the same "merge" overhead as regular patterns.

This effort may deserve a document of its own.

Thanks for pointing out the search process for selecting all the quilts!

[TomD.inPDX]

I never knew about that "history" "all" switch. No wonder I was getting zero results for my search attempts

[pnos]

try like this

[lkasch]

Hey Pepa Nos.

Thank you for your input, and making the video. Your sollution is actually how we make the oversized sketch pattern, the problem is just making the slanted pattern fit inside a box.