Controlling parts at assembly level ?

[Randy1111]

I've recently moved to a company that is looking to switch from 2d acad to the 3d world, using either solidworks or inventor.

I have used solidworks in a different industry so my experiance is not fully relevant in certain areas.

We produce an assembly, made of about 8 parts, in maybe 20 styles. Within each style, the individual parts are almost always a bit different, so configurations dont seem the best route.

I want to make up a template assembly file, complete with drawings all fully dimensioned (1 for each 'style'). And have a single design table inside each assembly, or a single external excel file, that holds every variable.

The only way I've accomplished something similar previously was by having the design table generate a skeleton sketch of construction lines, axis, and planes. Then have each part fully constrained to the sketch.

Change the design table, the planes move, all the parts move with it.

Is there a better way to control each individual part size or is this about the only way since you cant actually put part dimensions in an assembly design table? Does Inventor have the ability ?



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Jarery

 

[dezignstuff]

you might be looking at a KBE system like RuleStream. It's pretty pricy, but it definitely can do what you ask with the help of SolidWorks.

Or you might be able to create a home-grown configurator in excel. Make a design table with a bit of an interface with toggle switches and user data entry with validation.

I think what you ask is "almost doable", which means that the fully dimensioned prints are probably not going to happen unless you can get away with dimensioning planes or existing sketches. It becomes more difficult if you need to swap out parts, but not impossible. The better you are at excel, the more likely you are to be able to make this happen.

Matt Lombard

http://www.Dezignstuff.com

 

[SBaugh]

http://www.scottjbaugh.com/Design_Portfolio/SW_Models_w_DT_and_VBA/SS_Article.zip

I used in-contexted parts to planes in the assembly and changed the Assembly DT and the entire model updated. The article I wrtoe many years ago talks about that and how I accomplished this along with this article:

http://www.scottjbaugh.com/Design_P...and_VBA/In-contexted_Plane_mated_assembly.zip

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[Randy1111]

Thanks Scott

Looks like your approach is similar to my conclusion as the best way. I just didnt add the vba and fancy gui for inputting the changes, i'll definatly have to try that.

The ability to directly control part sizes from an assembly without a 'workaround' is a negative for me. But I like your approach better than the master/assembly/part external excel files, since each has to be opened in order to refresh changes. If you ever forget to open each part and then its design table, it doesnt update. So then you have the potential to send out drawings with the wrong dimensions. Thats a HUGE shortcoming to solidworks for me.

I'll have to evaluate Inventor and see how it compares.

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Randy

 

[CorBlimeyLimey]

SW2006 has DriveWorks Express embedded. It may be able to do what you are trying to do.

http://www.javelin-tech.com/main/products/driveworksxpress.htm

We produce an assembly, made of about 8 parts, in maybe 20 styles. Within each style, the individual parts are almost always a bit different, so configurations dont seem the best route.

Without knowing the extent of "a bit different", that actually sounds perfect for an assembly Design Table controlling configurations of parts. Do you mean that they are customised for each client?


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[handleman]

Sounds like you're (rightly) headed in a different direction, but if you ever need to open and update a bunch of design tables, you can use the macro in faq559-1231. It updates the design table for any open document, including all parts and subassemblies that don't have their own window but are loaded to memory because the assembly is open.

 

[Randy1111]

"a bit different" means a few of the parts have almost unlimted combinations of dimensions. The assembly is a pulley and something like the shaft is never the same as one done previous.

My understanding of configurations is they work great with a finite number of sizes, like a few hundred or less. When you have 1000's of sizes, its not the best approach.

That macro will definatly help alleviate the problem i mentioned earlier of having wrong data untill each parts design table is opened and updated if i go that route. I guess I just hate having to rely on workarounds for something I feel should be core essential in the program to begin with.

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Randy

 

[J-C]

Randy, can you post a pic? Might help us help you.

There are two basic ways to go about this. Use a master part file with most of the design done as multiple solid bodies in one part file. You basically model everything in one file....this works ok if there aren't too many parts and features as the tree can get complicated. The solid bodies can then be saved out as separate parts and assembly automatically created then you can bring and assemble other parts like nuts and bolts and other non parametric parts. It's all still linked back to the master part file though so you change your dimensions from there.

The other method is "in-context assemblies. Basically you can create layout sketches in the assembly that are a "skeleton" of the layout. Then create new part files in place and linked to the assembly layout sketches. Most all controlling dimensions are in the assembly and the parts just follow along. Down side can be performance and rebuild times but it's automated.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP4.0 on WinXP SP2