Attached is a part I made that works, but does have an arrow in the pattern sketch.
I can't determine what is causing the error in the pattern sketch. I think it's because some of the pattern being cut does not have material to be cut from, but I don't use patterns much.
I also wonder if this is creating the part to work slow or if it really is just a heavy parts and there is nothing I can do about how CPU heavy the part is.
One planes controls the part with a 1" and change incrament that matches is the expanded metal we purchase.
If you edit your sketch, you will see that there is some occurence on the right that will not remove material.
To solve this:
- In sketch, click to select pattern.
- On the commande ribbon, click on the left most button called "Select - Stagger Options".
- In the Stagger Options" dialog box, uncheck "Include last column".
- Click on Ok.
- Exit sketch and let Solid Edge recompute.
Problem should be solved.
If you RMB click on the pattern in the feature tree, then select "Investigate Error" it will tell you that there are several instances in the pattern that are not adding/removing material. So edit the sketch and you can either manually suppress those instances or use the suppress region, then select the square that made up the pattern which will suppress all the instances inside that region. Wonderfully thought out, you can flip and it will suppress all instances outside the region. Kudos to the SE developers on that one!
@Michel_Corrivbeat me to it. I did not see that option I will have to remember his solution, good to have multiple options.
I cleaned that part up, its not as heavy on the computer any more with the error removed.
I have one detail left to figure out. Depending on the increment used, my sketch on the top of the part that's used to clean up what the pattern can't handle is not in the right place half the time. I may need a second file with a different sketch to handle those cases of how long it is (every other plane increment). I'm wondering if I can make a conditional mirror or transpose of that sketch or if any have other thoughts for that case to keep the source file for this set of parts a single file.
I can't open the file right now, but looking at the screenshot, wouldn't you lock the pattern to the edges of the tab, so it doesn't go outside the part? Just a thought.