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pattern driven component in part

Question asked by Rik Harberink on Feb 2, 2016
Latest reply on Dec 11, 2018 by Bjorn Hulman

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We put PEM nuts&studs in our sheetmetal plates.

By now we have the plate as a part, the PEM nuts as parts and all together assembled in an assembly.

I put the nuts in the assy with the pattern-driven component using the holes created with a hole-wizard (part-level)

But because the nuts are pressed in the plate, this forms a solid/single part (like a weldment)

So I thought that this would also be good if drawn as a multi-body part (or weldment).

When placing the nuts, I constrain one nut and want to use de hole-wizard sketch and sketch-pattern to put the others in.

But then 1 nut to much will be placed (at the original hole)

Is their a way to use the pattern driven way, like in an assy?

I know a work-around is to delete the extra body... But it would be nice if it worked like the pattern-driven way.

Rik

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Timothy Taby Feb 2, 2016 9:28 AM
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Do it as an assembly. Make your part and put the first hole in and then put the rest of the holes in using a pattern (any kind of pattern will work).

Assemble the Pem fastener into the drive hole of the pattern, then under insert ----> component pattern ---> pattern driven, you select your component to pattern (your Pem Nut) and use the hole pattern as your driving feature (tip...to select it expand the tree for that part and select the pattern).
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- Daen Hendrickson @ Timothy Taby on Feb 2, 2016 10:26 AM
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  Using SW2014 SP5, it is unfortunate that the sketch-driven pattern within a part does not offer the "instances to suppress" option that it does in an assembly. Deleting the additional body at the seed location may be the cleanest method - perhaps add a comment to the delete body feature explaining its need.
  
  Daen
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  - Daen Hendrickson @ Daen Hendrickson on Dec 11, 2018 10:54 AM
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    An alternative is to create a sketch to drive the pattern.
    
    Make the hole wizard location sketch visible.
    Create a new sketch on the same plane as the hole wizard sketch
    Set your selection filter to Sketch Points
    Window select all the sketch points in the hole wizard location sketch
    Convert entities
    Either delete the seed location sketch point now, or perform a ctrl-select on it one step back before converting entities
    Remember to set your selection filter back to select all
    
    Now you have a parametric sketch with points at the hole wizard locations except for the seed location. You can use this to drive your sketch driven pattern without the need to delete the seed body. The downside of this method is that changes to the quantity of hole wizard holes does not update in this sketch - it must be done manually.
    
    Daen
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    - Bjorn Hulman @ Daen Hendrickson on Dec 11, 2018 11:07 AM
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      Note with this method, adding or subtracting entities in the hole wizard will not automatically update the number of inserts. and if a point is removed you will get a dangling entity.
      And at this point the use of the hole wizard becomes academic. You may as well cut extrude the hole, and in that sketch add sketch points of all other hole locations. You can then sketch pattern the hole from it's own sketch. Plant the seed insert on the original hole and sketch pattern the insert using the same sketch also.
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Bjorn Hulman Feb 2, 2016 9:38 AM
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Hi Rik,

I've always done it as a part and assembly as you describe, with hole patterns at part level and derived patterns at assembly level. An assembly will allow you to add a BOM to your drawing so the fabricators can quickly see how many of each fastener goes in.
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Rik Harberink Feb 2, 2016 9:47 AM
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I always did this as an assy, but now I want it as a multi-body part.
My customer uses the same partnumber for assy and part. (Which I think this is wrong...)
And so I want to make it in a single part, like a weld-stud in a weldment.
Than you have only 2 files (1 part, 1 dwg) instead of 4 (1 part, 1 assy, 2 dwgs)

I can use a cut-list for counting the fasteners.
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- Bjorn Hulman @ Rik Harberink on Feb 2, 2016 9:55 AM
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  Fair enough Rik, if that works for you. Can you not exclude instances? Otherwise simply do a delete body on the duplicated body.
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- Timothy Taby @ Rik Harberink on Feb 2, 2016 9:55 AM
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  The best way to do it is the assembly method plain and simple. What difference does it make if you have 2 files or 4 files?
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Sergio Monti Dec 7, 2018 7:05 AM
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Hi Rik, I have the same problem. Have you found a solution?
I also create everything that is welded together as a single part because we buy the welded part from our supplier and I don't want welded nuts appear in my BOM.
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- Greg H. @ Sergio Monti on Dec 7, 2018 9:50 AM
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  You could always exclude the nuts from BOM from the assembly. But if you prefer that it is made as a multibody part, it can be done, just with more steps.
  
  Instead of a sketch driven pattern, you would use a linear pattern (assuming linear). Then, assuming you want the pattern driven, you would then link the values to either the hole wizard sketch, or pattern values, depending on how the holes were created.
  
  Since you are using a linear pattern, you can even skip instances like I did in the upper middle.
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Glenn Schroeder Dec 7, 2018 10:04 AM
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1. Set up global variables for the pattern distance and number of instances.
2. Don't use the sketch pattern for the Hole Wizard. Create a single instance with the Hole Wizard and use the Linear Pattern function to create the additional holes, using the global variable values for distance and number of instances.
3. Place the first nut at the same location as the first Hole Wizard hole.
4. Create a second linear pattern for the nuts, using the same global variables (making sure to de-select "Features to Pattern" and selecting "Bodies to Pattern" instead).
I realize this isn't perfect, but it should work. If the patterns need to be edited just edit the global variables and both patterns will update to match.
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Sergio Monti Dec 7, 2018 10:55 AM
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Thanks Greg and Glenn, I appreciate your advice. I really don't use it very often. It happened few times. I tried sketch driven pattern at first, but there was something wrong with the hole callout when did the drawing, then I ended up doing two separate identical linear patterns. I understand that link parameters is the right way to do it, but I didn't because not worth it at that time.
It isn't a big issue for me, I can cope one way or the other, I'm only saying that shouldn't be difficult for SW software engineers to add in parts this function already available in assemblies.
For sure I'm not going to use an assembly to do a welded part - multibody parts for welments was one of the main reason we choose Solidworks amongst the other CAD software!
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- Greg H. @ Sergio Monti on Dec 7, 2018 11:34 AM
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  Sergio Monti wrote:
  
  I understand that link parameters is the right way to do it, but I didn't because not worth it at that time.
  
  Not over complicating it is the right way to do it.
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Dwight Livingston Dec 10, 2018 4:45 PM
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Rik

I would mark Daen Hendrickson's reply as correct. You can, indeed, use a Hole Wizard sketch to pattern the insert bodies, just as you would in an assembly. Sure, I don't know why Solidworks repeats the seed body, but it is simple to delete the extra body. Should we ever adopt a multibody method for sheet metal parts with inserts (we have been thinking about doing just that) then we'd do it that way.

Dwight
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