How to pattern a feature by referencing another feature's pattern

[ssmithdigilab]

Is there an option to create a reference pattern in solidworks?

For example, I create a cut on my part and then create a linear pattern of that cut (4 instances). Then using the hole wizard, I place 18 holes on the first cut. I then want to pattern the holes by referencing the pattern of the cut. There are 4 instances of the cut, so there will be 72 holes in total. It would take quite a bit of time to individually place 72 holes on this part. 18 is bad enough!

I know that in Pro/E when you chose to pattern a feature you had an option to create a reference pattern. I can't seem to find anything like that in Solidworks.

 

[CorBlimeyLimey]

Move the HW feature above the 'cut' pattern and then include the HW feature in the 'cut' linear pattern

 

[AnnaWood]

Or just move the hole wizard feature above your linear pattern and include it in the pattern with the cut feature.

I am assuming the holes are related to the cut and SW will not allow you to move it above the cut. If this is the case the HW feature is considered a child of the cut feature.

Cheers,



Anna Wood
Core i7 EE965, FirePro V8700, 12 Gb RAM, OCZ Vertex 120 Gb SSD, Dell 3008WFP 30" Monitor
SW2010 SP2.1, Windows 7 x64

http://www.solidmuse.com

http://www.phxswug.com

 

[mjcole]

You can also add Rounded or Fillet features to a pattern feature and if you suppress the round it won't affect the pattern SolidWorks will just pattern the selected features if they are in the active model.

This Blows Pro/E's reference pattern out of the water. Pro/E's reference patterns are nice but make a super ugly Feature Tree and if you suppress a feature the entire pattern gets suppressed.

Michael

 

[ssmithdigilab]

Thanks for the help, everyone. The problem was actually a little more complex than I described, because I figured making it simpler would help the solution to come to the surface quicker.

I'll describe how this part is actually made...

There is a cut, then below that there is another cut that cuts away some of the material of the 1st cut. Then the 2nd cut is patterned 4 times within the 1st cut. Then there are 4 holes that reference the 1st seed of the 2nd cut. Then those holes need to be patterned referencing the pattern of the 2nd cut. Then after that, we need to pattern all of that (the 1st cut, the pattern of the 2nd cut, and the holes and pattern of the holes) 4 times across the entire part.

The problem became really simple when I saw "include it in the pattern with the cut feature". You really don't need to move anything in the model tree. All you have to do is make all of the features first, and then go back and pattern after. While creating the patterns, select all features that you want to go with the pattern. I didn't realize you could select multiple features with a pattern, because I usually highlight the feature I'm patterning in the model tree first and then select the linear pattern command. You're right, this does blow Pro/E's reference pattern out of the water.

Another question I have, though, is about groups. Is there any way to group features together? Sometimes the model trees get ridiculously long with all of these patterns, etc.

 

[CorBlimeyLimey]

Features cannot be grouped as such, but they can be placed inside a Folder within the FM tree.

 

[wooska]

Where I miss the reference pattern from Pro/E is more in assemblies. If you pattern something in a subassembly (not a feature, but a component) you cannot reference that pattern in the top-level assembly. Pro/E would default to a reference pattern, which made life a lot easier when assembling complex systems.

 

[ssmithdigilab]

One thing that I just noticed is the hole callout qty doesn't update with a sketch driven pattern. In my case, it's actually necessary to have a sketch driven pattern because the 4th instance has a slightly different spacing than the other 3 instances.

When I originally did a linear pattern, the hole qty (called out on the drawing) updated based on that linear pattern, but when I changed to using a sketch driven pattern, the hole qty in the model was correct, but the hole qty called out on the dwg reverts to the original qty in HW feature. Is there any way to get that hole qty to update to the total qty of holes on the part based on the sketch driven pattern?

If not, is there a way to modify the spacing of one of the instances in a linear pattern?