In a weldment, how can I pattern the hardware? The hardware was placed using the insert>part command.
I did try using both feature and body in the pattern. Would let me select them either way.
No, I don't want an use assembly.
Jake Irvin wrote: My issue has to do with being able to select the hardware items in any pattern, rather than needing a specific pattern and not being able to select it. I did try the sketch pattern option (with my hole feature sketch). Same inability to select the hardware items.
Jake Irvin wrote:
My issue has to do with being able to select the hardware items in any pattern, rather than needing a specific pattern and not being able to select it. I did try the sketch pattern option (with my hole feature sketch). Same inability to select the hardware items.
Uncheck feature/faces first and then check bodies in order to select the bodies. Then you can use linear pattern in case holes are equal distance, sketch pattern (you would need to create an additional sketch with points) or table driven pattern.
Can you select a "Sketch Line" ?
Do you mean try to pattern based on the sketch in the feature? This doesn't seem to work.
Again not sure if this is what you mean.
Try to add a sketch line to one of the existing Parallel Planes...
I do appreciate the help, but not sure what you are saying. Any videos or articles on what you are saying?
It works for me if I do a pattern-driven pattern, as long as all the holes are either:
part of a pattern,
all made in a single Hole Wizard feature.
In your model, the holes all appear to be separate features, so Solidworks doesn't know they are related.
I would change the first Hole Wizard feature so it had all 3 hole positions in its sketch, delete the other 2 Hole Wizard features and pattern the fasteners in a Pattern-Driven Pattern, using the hole wizard feature as the reference.
SW 2018, SP5
Holes should be good as shown below. I don't see the pattern drive option... may be a weldment limitation?
Yes, it's part environment limitation, not weldment.
It's not a feature I use much, and I'm at World now so I can't test it, but I think you can create a sketch, with sketch points where you want the hardware, and then use a Sketch Driven Pattern (I think that's what it's called).
As Igor says, I think you can't do it in a Part, only in an assembly.
WINNER! Yep, had to deselect. I don't recall having to do that before. New thing is 2019?
Jake Irvin wrote: WINNER! Yep, had to deselect. I don't recall having to do that before. New thing is 2019?
No it is an old thing now, may be 2016. And actually you do not need to deselect but simply select one of the two check boxes.
No, asDeepak Gupta said, it's been that way forever. See Why am I having problems with the Pattern (or Mirror) feature in my Part?
I'm curious why would you be inserting tool box parts at the part level? Assembly would be way easier
Trying to set up a structural starter part with weldments. Trying to keep it as simple as possible.
Jake Irvin - Sometimes simple is harder downstream - how do the bom's and custom properties work in that type of environment??
assemblies are pretty simple... doing it your way you've negated any custom properties in the hardware and now have to enter them again. part numbers/descriptions.
Also if for some reason you need to change hardware you;d have to do this all over again. Just my 2 cents.
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