How to mate multiple parts efficiently 3

[cadcoke5]

I have a number of brackets and other similar types of shapes which need to be mated to an assembly. I am trying to do this without having to create each mate one-by-one. Smart mates are not viable for this type of part... a bracket.

I already have made copies of the parts (by using CNTL-drag to copy them). I had hoped to be able to select faces from the various copies, then the one face they all mate to, and then select Mate. But, it appears you can't select more than the two faces which must mate.

If I could copy the parts, with the mates copied as well, that would do the job also. However, this doesn't seem to be available. I realize that it is not viable to do such a thing if the original were fully constrained, since the two parts would end up on top of each other. But, in my case, I only have the original partially constrained.

Any ideas on how to deal with this efficiently?

Joe Dunfee

 

[handleman]

If there is any regularity to the arrangement, the ideal is to use component patterns. Other than that, what version of SW are you running? If it's 2007, search help on Muli Mates.

 

[JMirisola]

What version of SW are you using? SW '07 allows for the mating of multiple parts to one part. Also, hold down the 'Alt' key for smartmates while dragging. By doing this, you can easily create a coincident and concetric mate at the same time.
SW '08 allows for the copying of not only the part, but the mates as well.

Jeff Mirisola, CSWP

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[cadcoke5]

Sorry, I really should have stated the release when I first posted. We are on 2006, and are unlikely to upgrade until this particular project is done.

Thanks for letting me know about the features in the more recient versions. I will keep them in mind when we upgrade.

Joe Dunfee

 

[ShaggyPE]

If there are mounting holes that the brackets are attaching to you may be able to use a "feature driven" pattern in the assembly. If your holes were created with hole wizard, or if they were created with a feature pattern, this technique will work. If one bracket attaches to multiple holes, you will need to be a little creative with the way you create the component pattern (i.e. skip instances). This method can be used as far back as SolidWorks 2001-ish.

-Shaggy

 

[cadcoke5]

Thanks again for the suggestions... even if I don't use them now, they are things to keep in mind for other projects.

In my case, the item is an L-shaped bracket that mounts a plate to a T-Slot type aluminum exrusion. I am not using any holes for mates at this time (though some will eventually be drilled).

Joe Dunfee

 

[Updraft]

Joe,

You have some good advice here. Shaggy's recommendation to use feature driven pattern is a good one that too many folks don't know about (a star for you, Shaggy).

I would also like to offer some ideas:
1. If you are mating a hole to a hole then instead of Ctrl-drag to copy/drop them within the assy, instead have two windows open - the assy and the part you want to add. Grab the part by picking on the hole edge that represents the concentric and coincident surfaces, drag it to your assy window and drop it onto the mating hole. This simple action makes it very easy to add the part and two mates in one smooth motion.
2. Use subassemblies. Make a subassy of a bracket and all the fasteners that will go into it. I even make subassemblies of a fastener/washer and use that out the ying-yang. Now you can use the bracket/fastener subassy with a net of fewer mates than if everything is at the one level in your final assy. It has been awhile since I've done it, but you should also be able to dissolve the subassembly into the top level assembly and keep the mates. Personally, I HIGHLY recommend using as many levels of subassemblies as possible to reduce the overall work and keep the tree more manageable. It is a dream to perform adjustments with these subassemblies. About the only time I dissolve these subassemblies is if it is required for a flattened BOM, which I resist. Did I recommend using subassemblies yet?
3. You can use configurations of subassemblies, such a a bolt/washer/nut combo where these are different sizes AND with the nut at different distances from the washer. Design Tables RULE!
4. Combine the use of subassemblies with the feature pattern. My practice is to make a seed feature, such as a hole, a different color from the part. I'll mate the first subassy (bracket and fasteners in this case) to the seed hole (easy to see because of its different color) then pattern the subassy to follow the feature pattern of holes. Awesome stuff here - speed, accuracy of components, ease of maintenance (change), etc.

I hope this gives you more ideas to shorten your work.

- - -Updraft

 

[polykracker]

This might apply to Updraft's comment #3. At our work we have to flatten BOM's which results in way to many mates (1000+) in the assy's and thus bogs down our systems. I wanted to toss out this idea good or bad.

1. For the SW BOM type use PARTS ONLY and keep the sub-assemblies of screws/washer/nuts in your upper level model.

2. For all the assemblies that you want to remain as a single item, create a design table in the assembly and ADD the column header $NEVER_EXPAND_IN_BOM and set all the columns to Y (yes)

In the drawing it will count the number of screws washes etc. but not drill down and list all the parts in your 'selected' sub-assemblies. Thoughts?

 

[sldwkmin]

Look up "mate references" in the help menu! If it's a part used multiple times this is the perfect solution.

Cole M
CSWP, CSWST, CSWI, CPDM
HP XW4300, 3.4g proc, 2.5g RAM, ATI Fire GL 3100
Dell M90, Core 2 Duo, 2g RAM, Nvidia Quadra FX2500M
Equus (custom), P4, 3.4g proc, 3g RAM, Nvidia Quadro FX3400

 

[cadcoke5]

Thanks guys for the replies... but the message was started back in Oct. I don't recall the part.

Joe Dunfee