assembly feature patterns

[KSHansen]

I have an assembly with patterned components. I put an extruded cut feature into the first component, and want to pattern it as well, but it won't pattern. The sketch lights up when I hover over it in the tree, but the cut doesn't appear.

So first of all, you can't do a component-driven feature pattern?

Second, you can't do a feature pattern in an assembly if any instances cut into a new component?

We drill these in assembly, I just want to be able to vary the number of components I show in my drawings or assemblies. Am I going to have to create a subassembly for the component so I can put holes in it instead?

[AlexLachance]

I have an assembly with patterned components. I put an extruded cut feature into the first component, and want to pattern it as well, but it won't pattern. The sketch lights up when I hover over it in the tree, but the cut doesn't appear.

So first of all, you can't do a component-driven feature pattern?

Second, you can't do a feature pattern in an assembly if any instances cut into a new component?

We drill these in assembly, I just want to be able to vary the number of components I show in my drawings or assemblies. Am I going to have to create a subassembly for the component so I can put holes in it instead?

You can do both, you just can't do them in the same feature. One pattern will be used to repeat components, the other pattern will be used to repeat the extruded cut feature.


To your second question, I'm not sure I understand.

[KSHansen]

Right. I used Assembly Feature > Linear Pattern

Why are the subsequent patterned cuts almost nonexistent?

[josh]

You may have to edit the feature scope to include all components instead of "selected components"

[AlexLachance]

Right. I used Assembly Feature > Linear Pattern

Why are the subsequent patterned cuts almost nonexistent?

Did you create 2 Linear patterns, or only one? Because you need to create a pattern to repeat the components and a pattern to repeat the cut. Also, as Josh said, you might need to edit the feature scope to include the desired components in your list of selected components (or you can go with all components if that works for you too)

[KSHansen]

You may have to edit the feature scope to include all components instead of "selected components"

I'm not sure what that means. I've looked, but I can't find any videos on assembly feature patterns. At least not any that go into that kind of detail. Everything is about component patterns.

The Solidworks help just says:

To create an assembly feature pattern:

1. Create an assembly cut or hole.
2. Do one of the following:

• Click one of the following on the Features toolbar:
  • Linear Pattern
    Circular Pattern
    Table Driven Pattern
    Sketch Driven Pattern
  Click Insert > Assembly Feature, and select one of the following: Linear Pattern, Circular Pattern, Table Driven Pattern, Sketch Driven Pattern.

3. Set options as needed in the PropertyManager.

It reminds me of a Monty Python sketch where they were teaching how to do things. Like, here's how to play the flute: You blow in here, and you run your fingers up and down the keys!

[berg_lauritz]

Ahhh, great problems. Almost un-fixable in my humble opinion. I'll try to explain why it might fail randomly and how to maybe fix it. I cannot prove anything of it, so please take it with a grain of salt and if you find a fix - please let me know. Also.... I'm super mad about those problems:

• If you use ANY external references, turn on to show the update holders:

  

  now you'll see sometimes (not always) things like this:

  

  2022-07-06 15_28_14-Window.png (11.58 KiB) Viewed 1519 times

  which you will now be able to re-order. It is important to order them 'in the correct order'. I.e. if Part A needs and update AFTER Part B you should order it in the feature tree like that! It might fix some issues for you.
• EXPAND the mates folder for ALL PARTS. Sometimes it will show you an error only after you expanded the mates folder! Even better: It will show you an erroneous mates folder even if it's EMPTY. Usually this happens only if the part has OR had an external reference in that assembly! The only way to fix this is to re-insert the part. The reason seems to be that there is a seemingly unchangeable 'inserting order for parts & features' stored within the assembly. If you re-insert the part it will get moved to the end of the inserted order and suddenly everything works again.
• Try to not link anything from assembly feature #1 to assembly feature #2. The calculation order is not always what it seems to be. Often times SolidWorks seems to calculate feature2 before feature1 within an assembly (i.e. feature1 creates an edge that feature2 uses - usually causes issues down the line). If they do not depend on ANY other feature it seems to be stable.
• Try to fix ALL components in place and remove any mates from the feature tree. Mates seem to be connected to those issues because they are calculated multiple times within the assembly.
• Get rid of any virtual component. They are loaded somewhere in between, because they reference the assembly.
• Try this tool from codestack.net and delete hidden features. But be careful with it - it might mess up everything!
• Your failing part might look correct but it is not. To be sure that it works you need to open the part, access every single feature one after another and hit OK. Only then you can (mostly) be sure that the part is 100% correct. You might be surprised that some features suddenly 'flip' after you do this (reverse direction on a base-flange, cut-extrudes 180degrees turned...). THEN you go back to the assembly & fix everything and suddenly it might work again.
• Now here comes my least favourite but most stable solution: Move the features into two different assemblies (Promote the assembly in the BOM if necessary). This way feature A will get done before feature B is done.

easy peasy, lemon squeezy

Edit: Totally misunderstood the problem. I'm sorry. Do it as @AlexLachance mentioned.

[AlexLachance]

I'm not sure what that means. I've looked, but I can't find any videos on assembly feature patterns. At least not any that go into that kind of detail. Everything is about component patterns.

The Solidworks help just says:



It reminds me of a Monty Python sketch where they were teaching how to do things. Like, here's how to play the flute: You blow in here, and you run your fingers up and down the keys!

This is what he refers to as the feature scope. For instance, in this screenshot, the cut applies only to 2 components. I want to pattern the component, but I also want to pattern the cut. Right now, the cut is only applied on the original instance and the pattern isn't created

Picture to show the cut with feature tree

Now the pattern is created, but the cut isn't on there still, because the components weren't selected previously.

Add them to the feature scope previously spoken

et voila

[KSHansen]

You may have to edit the feature scope to include all components instead of "selected components"

Ah, I got it, the feature scope in the extruded cut feature. I was looking for feature scope in the pattern. So yes, this worked - whenever I change the number of components in my pattern, I have to go into the cut feature and update the scope to include all instances of the component. This is a far cry from Creo's three clicks to do this pattern.

Edit: Thanks, Alex! I figured it out while you were making that reply.

[DanPihlaja]

You might be better off making the cut at your part level and using configurations to suppress or unsuppress the cut instead of patterning 2 things at the assembly level (the part and the cut).

[AlexLachance]

You might be better off making the cut at your part level and using configurations to suppress or unsuppress the cut instead of patterning 2 things at the assembly level (the part and the cut).

If it's a part that is standard, that could be a trouble-maker. The feature would need to be supressed on the original config and not the new one, or all the instances of the part that are inside existing assemblies would be updated to have the feature that isn't necessarly desired.

It could also cause people to insert the part on the wrong config.

[TTevolve]

I try not to do holes at the assembly level unless I have to, it can tend to have unintended consequences

Alex, what is that assembly of?

[KSHansen]

You might be better off making the cut at your part level and using configurations to suppress or unsuppress the cut instead of patterning 2 things at the assembly level (the part and the cut).

If it's a part that is standard, that could be a trouble-maker. The feature would need to be supressed on the original config and not the new one, or all the instances of the part that are inside existing assemblies would be updated to have the feature that isn't necessarly desired.

It could also cause people to insert the part on the wrong config.

If I was using the model to drive BOM and manufacturing, I would have to put holes in the assembly, because that's how they do it in the plant. But I'm not, so I can really model it any way I want. It might be easier to do a save-as of the original assembly and components, and then put the holes in the component.

[AlexLachance]

I try not to do holes at the assembly level unless I have to, it can tend to have unintended consequences

Alex, what is that assembly of?

It's a trailer assembly at the suspension installation level.