Assembly/Drawing Configurations and Mate Best Practices 2

[Jieve]

Hi, I'm wondering if I can get some input on assembly configuration mating best practices.

My process generally goes like this: say I have an assembly with 20 individual parts. All parts are properly mated, but then I decide to change one part completely. I open the part and create a new configuration. If I decide to change the entire shape/design of the part, then I will usually suppress the unnecessary sketches/features from the default part and start with a new sketch. When finished I create a new configuration in the assembly. When I re-configure the part in that assembly, I get a bunch of mate errors, because the original faces/mated features no longer exist. I then suppress those faulty mates in the new configuration, and create new mates.

My questions:
1) If a new version of a part is very different from an older one, is it generally better to just completely create a new part file, or is my configuration method of suppressing/copying/adding new sketches and manipulating features reasonable and more common practice?
2) Is my method of suppressing the faulty mates and adding new ones for a newly configured part good practice? And if so, do you organize those separate mates in any way, for example by putting them in separate folders? In the past I would try to correct those faulty mates by re-mating the new faces, but doing this messes up the mate in the previous configuration, correct?

I've noticed in the past that I've had seemly random mate issues pop up, where in certain configurations suddenly things wouldn't be mated properly and I wasn't sure why, so I'm trying to see if my methods are correct. Thanks for any input!!

 

[hendersdc]

If you are trying to maintain revision control of the part or assembly then it is good practice to have no suppressed features or sketches in the parts or suppressed old parts in the assembly, that way when someone is looking at the files for revision C there is no way anything from A or B could be in there that wasn't intended to be carried over. Configurations just mask the problem not to mention I believe the default state is for new features to be unsuppressed in all configurations which could become confusing. I would think that all these configurations are drastically increasing your part size and rebuild times as well.

 

[TheTick]

Sounds like you're suppressing old and creating new when you should just be changing things.

Configurations for revision control is just a bad idea. It wastes way too much time. Usually it wastes a lot of people's time while one lone dingbat insists that it's pure genius.

Far better to archive old versions in an out-of-the-way place like a zip file.

 

[Jieve]

Interesting, thanks for the feedback.

I have been using configurations for one of two things:
1) because I have two different versions of a final assembly (say one with a different mounting type than the other), or
2) because in the design iteration process I am trying out different designs on a base part or assembly, and felt it was faster/less complex to make a new configuration than copying and creating an entirely new part, or assembly with new parts.

So what do you feel is the appropriate use of configurations?

And what would you consider a best practices way to deal with 1 & 2 above?

Thanks!

 

[ctopher]

I mainly use config's for variable lengths, heights, colors, etc.
If form/fit/function is different, it's a new part.

Chris, CSWP
SolidWorks '16
ctophers home
SolidWorks Legion

 

[natepiercy]

Jieve,
We use configurations in assemblies that can be assembled multiple ways, such as a bracket that can on the front or back of an arm. I personally have used configurations (well, Simplified Reps in Creo, but same thing) in tooling / fixture design, to show that a tool/cart/fixture works for multiple products. Showing all clamps opened vs closed, showing the part in the fixture with the appropriate clamps engaged, etc. If the model contains a cylinder or actuator, it may be useful to show the assembly when the cylinder is extended, then double-click to show it mid stroke, and double click somewhere else to show it retracted. I think this is exactly what you're getting at with #1, in which case I agree completely.

#2 though, If you're talking about something like changing a hex screw to a socket screw, that seems like a sensible alternative to replacing 3*N mates. If you're changing the design from a bolted to welded joint though, toss configurations out the window. I've only ever found configurations to be useful at the assembly level, personally. I second TheTick's suggestion of making a pack-and-go at whatever stage you want (for your records) and stuffing it a zipped Archives folder.

 

[MadMango]

For parts I use the "Save As Copy and Open" method when I am crunching through design iterations, adding a 1, 2, 3, etc after the name of the file. It is then easier and safer to use Replace Component instead of Suppress an unwanted part in the assembly. No Mate errors.

Configurations are good when something simple is a variable, like color, material, length or width. Trying to use it for revision control should be considered abuse. And as Tick alluded to above, it only takes one user that is not that knowledgeable or attentive in SW to destroy a model (part or assy) with configs.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[drawoh]

Jieve,

The basic design change rule is that you do not change form, fit or function on a given part. If form, fit and function must be changed, you create a new part or assembly. Note how a massively redesigned part does not necessarily affect the form, fit and function of the assembly. Production can assume that any part with a given part number will work in any assembly calling up that part.

If your revision of your assembly does not affect form, fit and function, you revise the assembly. With CAD, when you revise something, you should archive the original version somewhere. This is what PDM does.

If you change form, fit and function, you have designed a new part, which should have a new part number. You can do this by generating a new model and assembly. The old assembly still exists. You call up the new assembly on whatever it is that requires it.

Your other option is to add or increase the tabulation on your assembly drawing. This is supported in SolidWorks through configurations. The assembly drawing is simple enough. I see a table of part numbers and an explanation of the differences. I can kit for and build the old assembly, or the new one. SolidWorks supports BOMs with multiple quantities tied to the configuration. The configurations of the assembly model are more complicated. If you are like me, you use configurations to show assembly steps. Integrating an alternate part number could get complicated. Do you need the capability to select an assembly at the assembly drawing level? Sometimes, you do. If the new assembly supersedes the old one, this probably is not a good idea.

Attaching multiple assembly drawings to one assembly model is a very bad idea. Somebody wants one of the assembly drawings revised. The drafter/CAD operator does not know two or three other assembly drawings are affected by the model. The other two get affected and nobody knows about it.

If you have a confused, stupid way of doing things, SolidWorks will do an excellent job of modelling the confusion and stupidity.

--
JHG

 

[natepiercy]

If you have a confused, stupid way of doing things, SolidWorks will do an excellent job of modelling the confusion and stupidity.

QFT

 

[Jieve]

Thanks everyone for the detailed responses, some great information here.

Looks like I've been making things much more complicated than need/should be. I especially like the simple "save as copy" or .zip method for design iterations ... saves a lot of the grief associated with mate problems due to suppressing multiple sketches/features in multiple configurations.