How to aproach large and disorganised assemblies in solidworks ? 1

[marianw88]

Hello everyone,
I have just signed in and will get straight to the point with my problem. I am a recent graduate and just started cad position in small company which is mainly dealing with vehicle chassis assemblies. The problem for me at work are large assemblies of the vehicle chassis which have: under-defined elements, references broken, parts doubled, no naming on parts and overall is really difficult to work with, not mentioning it take ages to open, rebuild and change any off the features. Can you please tell me how to approach such assemblies in SolidWorks ? Is there any way to fix them quickly, automatically ? Any easy way to remodel them, apart from modelling each of the elements again and then put by mates together in new assembly?

 

[jassco]

Hi, marianw88:

You did not say what you need to do.

Best regards,

Alex

 

[marianw88]

My main task is to prepare the parts to be manufactured : open each part in SolidWorks than unfold, nest and send to laser to be cut, bend and folded. But my question is: is there any quick way to fix the assemblies which were modelled by someone else? There are two ways I see I can do it, one is start from scratch and remodel all parts and put them back in new assembly, other one, try to fix the assembly I got from customer by removing broken links, renaming the parts one by one, try to remove the references between parts ( which in some cases are real deep and 10 parts gets modified when you try to change one). Therefore I ask some more experienced modellers how they would do it if they would have to work with such assemblies.

 

[CorBlimeyLimey]

If your task is to create drawings suitable for manufacture, then do only that. Unless your scope of work is to "fix up" the parts & assys, leave everything else as is. If you inadvertently change a part, you (or your company) could be held liable for any costs incurred.

 

[ShaggyPE]

I agree with CBL. You have been tasked with one specific task. "Fixing" the assembly is out of your scope. I would recommend bringing the concerns up with the customer to notify them that the models are not fully constrained. One option to ensure the models don't get changed is to export the assembly to a neutral format (like parasolid [.x_t], STP, or IGS) and re-import it back into SolidWorks. This will make the new files "dumb solids" with no feature tree. You will then be able to unfold them as necessary. Run this by your customer though. Essentially they provided files for you to manufacture and your company quoted the task to do that. Anything beyond that could get you into hot water.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[marianw88]

Thanks for the advise, I will probably go for the export-import option, the assembly should be clear and easy to work with. I can save all the elements as igs files and assign them new names what should allow me create new assembly and list of components to be manufactured without missing anything.

 

[PatCouture]

I would use Parasolid as a neutral format because it should a lot more reliable vs IGS.

Patrick

 

[imagitec]

Are the assemblies created in house, or are they customer assemblies that your company is only manufacturing pieces of?

If you export and reimport everything, you're going to lose any intelligence, meta data, and associativity. That can cause pain later. If you're willing to consider that, I would do something much less drastic that retains much of the intelligence in the SolidWorks parts and models:

(1) Delete or suppress broken mates

(2) Fix components that are not defined in space by their mates. Start with the major components and go one by one. As you fix those components, you may find that components that attach to them are now defined in space. A good approach is to suppress everything, then start unsuppressing components one by one. Fix it in space by using "FIX" or by correcting broken mates & adding new ones.

(3) Use folders to logically group parts without creating subassemblies. Right click on a part in the assembly tree and select "Add to New Folder". Give the folder a logical name. Then drag related parts to the folder. You can then hide, unhide, suppress, and unsuppress complete folders.

I am also in the habit of renaming mates, especially critical ones. It sounds tedious, but if you know the keyboard shortcut for rename (F2; the same shortcut is used throughout windows, so it's worth knowing), it isn't. I use a naming convention like:

CartWheelTan2Stop

Renaming mates is especially useful for configuration-specific mates, which I prefix with the configuration name in ALL CAPS. These configuration-specific mates are often exclusive (i.e., if both are unsuppressed in the same configuration, they will overdefine the assembly).

 

[imagitec]

Never, ever accept SoldiWorks' offer to "Fix a mate" or "Fix a mate orientation". It will invariable get it wrong and break a dozen more mates in the process. SolidWorks' default assumption seems to be that the mate you're adding or editing (which would make it the most recent in a sense) is the correct one, and the others should conform. This is rarely the case. I honestly can't remember a case of SolidWorks default behavior being the correct or logical choice.

Select No and/or Ignore (I typically tell SolidWorks not to ask me again that session), let the new or edited mate be broken, then flip its mate alignment.

This comes up most often when:

(1) Replacing one component with another that looks similar but is modeled differently, so that the mate alignments aren't correct. For example, two screw models can look identical but have different "directions" and thus alignments.

(2) Fixing mates that have been broken because geometry changed. Again, the geometry (a hole, for example) may look identical. But it may have been put in from the opposite side, or it may have been modeled as a revolve where once it was an extrusion. This may prompt SolidWorks to ask you if you want it to "fix" the misalignment, breaking downstream concentric and coincident mates in the process.

 

[imagitec]

Large, complicated assemblies often have multiple configurations. It is important to understand the purpose of these configurations and set the corresponding mate options accordingly, or the result will be a maintenance nightmare.

There are two general uses for configuration:

(1) Show a subset of parts or a different subset of parts. You may do this to make it easier to work (e.g., large, busy models), to show different stages of assembly, or to show alternate constructions.

After defining the contents of the configuration, you may later decide that additional parts need to be added. You want to be able to simply unsuppress those parts and have their mates come along with them. To do this, the proper configuration properties are:

DO NOT CHECK "Suppress new features and mates"

DO CHECK "Suppress new components"

(2) Show components in alternate positions

This typically requires alternate, configuration-specific mates or configuration-specific values of mates (such as an angle or distance mate). See my previous post about naming such mates; it will make it easier to manage the assembly over time. Also, I don't recommend using configuation-specific values. If a part is at two different angles in two different configurations, it is much better to define two different angle mates, name them accordingly, and suppress or unsuppress in the corresponding configurations.

You can also reorder mates, dragging configuration-specific or other critical mates to the top of the mate list.

 

[MikeHalloran]

Don't try to 'fix' the _copy_ you got of the customer's assembly, because:
- You are apparently not contracted to do so.
- You will have to do it all again when you receive the next revision.

Given that the customer's model is apparently screwed up, you might request that the customer supply what you are expected to interface with in a neutral format. In any case, you should save a copy of what you got from the customer so you will have a defensible position in the inevitable arguments to come.

Instead of mating your parts to the customer's parts, which will change, consider fixing your parts in the vehicle's global coordinate system.



Mike Halloran
Pembroke Pines, FL, USA

 

[SnowCrash]

Lots of good advice here. I've been through this several times, usually as the only SW CAD operator.
First step is to create a backup of everything before you move forward.
Several of the work methods suggested will get you a stable model eventually.
Good luck.

--
Hardie "Crashj" Johnson
SW 2011 SP 4.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580

 

[KevinDeSmet]

Unfortunately, history based parametric MCAD software (this is not just SolidWorks) work in such a way that makes it far to easy to generate a complicated mess. I find assemblies to be even worse than the feature tree of a part, the problem with parametric assemblies is that mates as a concept as like a ticking timebomb and in-context relationships can become a spider's web.

Certified SolidWorks Professional

 

[EngineerErrant]

Another vote for Parasolid export/import, but more importantly, another vote for "don't do anything you aren't paid to do, and if you have to do something you aren't paid to do in order to do what you're paid to do, charge for what you're doing."

"Engineers like to solve problems. If there are no problems handily available, they will create their own problems." -Scott Adams

 

[DiegoLGraves]

We've often used a situation like this as a learning opportunity for ourselves and our customers. If you are new to SW you can learn from both the good and poor modelling practices. If you are an experienced SW user and can properly modify the parts and assemblies with a goal of training your customer to work with best practices you may help grow your company and your own reputation. You will become the go-to vendor. Personal contact with and advice for your customers will be appreciated when approached professionally and diplomatically.

Based on your comments I'd suggest that you take a limited approach to making changes. Make copies of what you need to change so you can compare your alterations to the original files and maintain design intent and requirements.

Regards, Diego

 

[rollupswx]

Unfortunately, history based parametric MCAD software ....makes it far to easy to generate a complicated mess.

What about all of these direct modelers the CAD press are hyping.
Try finding a problem in a model/assembly with no history of how it was created.

I estimate about 90% of what I see (from all MCAD programs) has serious flaws (by the designer) when I examine the history/constraints/dimensions (or lack of). Undimensioned stuff out to 8 decimal places, calculated bolt circles vs geometric bolt circles just a couple of the most common. I'm sure you guys and gals can generate quite lengthy lists of similar that would be hard to track down without history.

 

[Nella95]

I agree with MikeH in that - You will have to do it all again when you receive the next revision.

Don't fix or have 'them' fix it

Nelson



SW Premium 2011
64 bit SP4.0
Intel Xenon X5650 @2.67GHz
2.66 GHz 11.9 GB of RAM

 

[mjcole]

I think it's better to turn and run rather than approach those kinds of assemblies.



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