Inserting parts with same component origin 1

[Sparweb]

Hello
(Please forgive me for comparing SW to Inventor, I do not mean to offend)

There is a productivity tool in Autodesk Inventor called "insert at component origin".
It allows the origin of multiple parts to be aligned as they are being inserted. It goes click 1-2-3, inserting components with their mutually shared origins mated together in one step. This is tremendously handy and something I'd like to be able to do in Solidworks.

What is the equivalent in Solidworks? I am not dropping parts at the universal assembly origin.

To clarify (if necessary) say that I have a bolt and a washer modeled as parts with their origin under the bolt head and face of the washer. If their origins are mated, they would be perfectly mated to each other. I want to install them in a plate with a hole in it. It doesn't matter where the plate is. When I insert the washer into the model, in SW I have to mate it to the hole (normal enough). When Insert the bolt, however, I have to go through the process of mating it to the hole in SW. This should not be necessary, because all I really need to do is mate the bolt's origin to the washer's origin. I used to do this with 2 clicks. Populating assemblies with hardware is taking me and my coworkers a very long time in SW. I'm sure somebody has come up with a shortcut, but my Google powers are not turning up an answer.



No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
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[CheckerHater]

Read about "mate references" in SolidWorks Help and any other source available.

To populate big number of holes also check out "pattern driven component pattern" and, possibly "sketch driven component pattern"

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[handleman]

If you create a coincident mate between the origins of the two components, you'll get an option for "align axes", which will fully constrain the two to one another. Selecting the origins is a slight pain, because you have to do it from the feature tree (unless you use my reference geometry selection macro).

 

[Sparweb]

Copy with Mates.
Different workflow, but it is more efficient that what I was doing before.

No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[SwinnyGG]

Copy with mates is powerful, but if your base components are modeled correctly, Pattern-Driven Patterns are much more so.

It's also worth noting that pattern-driven patterns result in arrays of parts which are much lighter than inserting/mating each part individually- so if you're dealing with large assemblies that have a lot of fasteners, it may behoove you to investigate the pattern tools.

 

[Sparweb]

This feature was flaky in Inventor. I used it and broke models with it regularly.
I would have been leery to try to use it in SW until you seconded this recommendation from CheckerHater.
I would like to use a feature like this in several parts with numerous holes so I think I will investigate both ways of using it, next chance I get.
How tolerant is it of having the pattern sketch actually in the part model, when being used to place fasteners in the assembly model? Or of changing the part geometry after patterning in the assembly (even if the points are preserved, just moved)?


No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[CheckerHater]

Pretty well
You can have sketch in part model, you can create sketch in assembly model.
As you edit the sketch, the pattern will follow automagically
I do a lot of metal boxes; use patterns all the time, so I don't have to count my rivets.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[SwinnyGG]

I would like to use a feature like this in several parts with numerous holes so I think I will investigate both ways of using it, next chance I get.
How tolerant is it of having the pattern sketch actually in the part model, when being used to place fasteners in the assembly model? Or of changing the part geometry after patterning in the assembly (even if the points are preserved, just moved)?

Pattern-driven patterns are very powerful, and in my experience very robust.

You don't actually use the sketch- as long as the hole pattern at the part or assembly level was created using a pattern feature (of any type) or using hole wizard, it automatically detects the array of features and populates them. It's based on the pattern feature not on the actual geometry, so if you make a change and re-build the model at the part level (which might result in a change in a feature ID of one of the mating faces, for example) the assembly feature does not care- since it relies on the pattern feature it just gets re-populated at the next rebuild.

So you create your hole pattern at the part or assembly level, then populate one hole with parts, then create the PDP feature. After that, any changes you make to the hole pattern- you can make quantity changes, change the geometry, do whatever you want- at the assembly level it will re-populate the pattern automatically upon the next rebuild with no user input required.

 

[handleman]

I agree that feature driven patterns should be used just about whenever possible. However, I do have one word of caution about the feature driven pattern. Actually, about all component patterns in general. I've found that actually mating additional components to patterned instances of components can be unstable.

 

[Sparweb]

...I don't have to count my rivets.

Exaaaaaactly what I'm talking about! Thanks again!

No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[TheTick]

Throw the parts into a temporary assembly. Add the temporary assembly to the main and dissolve the temporary.