Designing in SolidWorks vs how manufacturing actually builds the product

Correct me if im wrong, but creating a model in SolidWorks the way manufacturing will build it is NOT the correct way to model. I say
this because im trying to figure out the best way to handle my problem. We dont use a unique numbering system, so all of our part numbers are sequential. If I am making a frame weldment with 8 legs, and the legs have 3 bearings on each leg, I make an assembly with the leg, bearings, tubing caps, and spacers the bearings mount to. Our manufacturing dept doesnt weld each leg separately, rather they like the entire frame weldment on 1 drawing with all components called out. If I designed the model like this, I would have to mate 24 bearings, caps, and spacers for each leg. Of course this is a headache in SolidWorks. With our current system, I have to generate a part number for this "imaginary" assy/weldment of the leg. This takes a part number up, plus it! might confuse people in the future who didnt create the model.
Can you give me your opinions on what the best way to go about this? What does your company do for this? What is the "best practice" for weldments/assys?
Any comments/suggestions greatly appreciated. Thanks.
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SW Monkey wrote:

The answer seems simple to me, but since it seems unlikely that a simple answer hasn't occured to you I presume that I'm probably missing something. But here goes anyway . . .
Why do you need to assign part numbers right up front while modeling? If you were to use descriptive names as a preliminary, then you could model up your subassemblies in the way that is most logical for Solidworks (creating your Mates as appropriate), then once you have your overall assembly together you simply Dissolve the subassemblies and number the parts logically as your manufacturing will build it. So -- tell me what's wrong with that. I'm sure there must be something.
'Sporky'
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I should have mentioned that we use Smarteam, and we need to assign the model a part number when checking the models into Smarteam. I could of course check it in as "Leg", but then I would have to make sure those are deleted later.
On Sat, 15 May 2004 22:00:20 -0400, Sporkman

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I agree with Mark's suggestions. Using assemblies and sub-assemblies for grouping and mating, then dissolving them later works good. Also, When I'm designing a new project, I work strictly off my hard drive. I use descriptions and date codes for part numbers. When the owner wants to see the latest, I show him what I have, and the date code helps to distinguish it from a previous version. Only released documents get checked into the vault. Best Regards, Devon T. Sowell www.3-ddesignsolutions.com
wrote:

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Well, I work in a team with 5 people. We are all working on the same major assembly, so we need to share files. Thats is the main reason I have to check files in, so others can use them.
As for dissolving mates in "imaginary" assemblies at the end of the design stage, what happens if you have to change a part in those assys that were resolved later on?
On Sun, 16 May 2004 06:08:57 -0700, "Devon T. Sowell"

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SW Monkey wrote:

I'd suggest maybe that your organization's priorities and your own negative approach to problem-solving are what are getting in your way . . . not the way SolidWorks works. If you've got to share portions of your design before the design is finished then you're going to run into problems no matter what software you are using. That's certainly the reality in a lot of companies and a lot of design work, but I really can't imagine how a software company can solve those problems FOR you. Can you? I CAN imagine how YOU can make changes to make things easier for yourself, however. Can't you?
Regarding having to change a part in the bogus assemblies after they are dissolved . . . I'd simply delete the outdated components and replace them. Use the original Parts and modify them if possible, and in that way you'll run into only minimal problem with Mates.
I don't mean to be hard on ya, Mr. Monkey, but aren't ya coming up with objections to solutions without trying to adapt the solutions to yer needs? If your project managers insist on seeing major assemblies together -- the result of the work of several people modeling separate portions of a project -- you must simply educate them in the realities of the software or find a way to share files without causing problems. Or both. In one such scenario I can imagine you assign a valid system part number to the major subassembly each of you are working on, and that part number doesn't change. When you draw together the various portions of the project in a top assembly you can simply use the Replace function and the top assembly updates accordingly. If you wish to have a contiguous block of part numbers for each portion of the top assembly, then assign blocks of part numbers to each designer. If your company's internal processes prevent that then call a meeting to discuss the problems. Be creative my friend. There are solutions all around you, but you won't find them by saying "yes, BUT ... ".
Mark 'Sporky' Stapleton Watermark Design, LLC http://www.h2omarkdesign.com
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Re: Dissolving In an assembly, sometimes I'll create a temporary assembly to group components that are locally positioned properly. Then, as a group, I'll move them to their new location. When the design is ready for a BOM, I'll dissolve this sub-assembly. Re: Mates I always fix every component in place and delete all mates when the assembly is finished. I use mates less and less as time goes on. I prefer to move components into position. Re: Teamwork I too, have worked in large teams recently. We decided that only released documents would go into the vault. We used date codes and each persons own initials to identify each persons components. The team leader's computer was made available to all team members and he was responsible for maintaining the master assembly. This method works quite well for us and avoids the hassles of using PDM Works unnecessarily. We got used to using SolidWorks Explorer and found it to be quite adequate. Best Regards, Devon T. Sowell www.3-ddesignsolutions.com
wrote:

drive. I

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Re: In Context Relationships I always break these as soon possible. They're so easy to re-establish, why have this extra baggage tied to each component? Devon
wrote:

for
to
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So, here's another example, this is how we really work. Say there is a component called widet-1. Say we want Devon, Tom, Owen and Chris to work on this part, each person to submit his own design.. widet-1_Devon widet-1_Tom widet-1_Owen widet-1_Chris Same part, different names, no problem. During the week, each designer submits his design to the team leader. The team leader inserts each part into a copy of the master assembly and then decides which design is the best. When the decision is made by the team leader, he renames the "winning" part to the correct name. We also use this method for assembly and drawing files. We use SolidWorks Explorer to copy and rename drawings, assemblies and parts into new folders. Best Regards, Devon T. Sowell www.3-ddesignsolutions.com
wrote:

wants
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Nice example, Devon. Maybe that'll turn on a light somewhere.
"Devon T. Sowell" wrote:

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Thanks Matt and Sean-Michael Adams for the response. I felt like Sporkman was giving me a hard time, maybe he doenst understand PDM? I should have responded sooner, but been busy. I stated we work in teams, but we dont compete to see who has the best design. That sounds a little silly to me, but its most likely because we would never do that here (i could see that being the way at companys who design products around customers ideas). Each person on our team gets a section of the project, for example, 1 person gets the frame, another the housing, etc.
Back to the subject, as stated, part numbers are cheap, we wont be running out anytime soon, thats why we use the system that we have now. I have tried changing part numbers later in the design, and what a pain in the azz it is with Smarteam. I will keep some of the ideas in this thread in mind.
Keep the opinions coming :)
Thanks.
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Let me just offer a different point of view. The other suggestions have their merits, but may also have some drawbacks especially in light of you using SmarTeam.
I think sequential part numbers are good, in fact, with a PDM system, they're almost essential. If you don't use them, there's a lot of maintenance that you'll have to do later with the names. I don't see a problem with what you're doing there. PDM systems work great with custom property description information. If you're dealing with a PDM system, changing part names is not a game you wanna get into.
Also, don't worrry about something "taking up a part number", cuz numbers are cheap, and if you have a good system, you won't run out in the next decade or so.
You're right to say that you don't always model parts the way you manufacture. I think you'd also be right to say that you don't make SW assemblies the same way you assemble on the floor, although it's nice if you can. If the end product that MFG sees is a sheet of paper, then who cares how the SW assembly was built? If you use the SW BOM on your drawing, just tell it to show the parts only, so every part will get its own part number in the top level assy. Assign a prefix or suffix for a part number to designate a "phantom". Certainly you have other assemblies that use parts that don't get shipped to a customer, like a model of a screwdriver to show how/where an adjustment is made for service / documentation purposes.
Dissolving sounds like a good solution, the only problem being what to do if you now want each leg to have 4 bearings? It limits the editability in the future.
Also, what do you do if you start using the SolidWorks Weldments? That may complicate things some, because the weldment is created as a multibody part.
Good luck.
Matt

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Matt,
I wanted to ask if you could expand on this a little. We're about to implement a new part numbering system without PDM but we should be prepared if it's something we add later. I've been reading this newsgroup a lot lately and you've always got good comments so thanks in advance.
Steve
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Thanks, Steve.
I do PDMWorks implementation for a living, among other things. I get to see how a lot of different companies do things. The customer in the end always makes the decision about part numbering, but I try to guide them by laying out strengths and weaknesses of various scenarios. I try not to give my honest personal opinion unless they ask, or if I see that they're doing something which is plainly stupid.
Definitely don't put the rev level in the file name. If you do this, you will create a file management nightmare. The only exception to this which might not be all that awful would be to put the rev in the file name for archived docs if you are not using a PDM system. Use "Save As Copy" or SW Explorer for this.
Everyone prefers to have file names be something readable, which has some sort of meaning. The only problem with this is that you are likely to make duplicate names, and "unique file names" is the #1 rule about SolidWorks file management. If you can use "descriptive names" and guarantee unique names, more power to you.
Another problem with descriptive names is when the function of a part is used in the name, and the part is used in multiple assemblies where the function may be different, for example a "locating bracket" may be used as a "support brace" somewhere else. Project names in the file name are not a great idea either because some parts may be used in multiple projects.
I have some people take the information that descriptive names and project names are not good to use individually and somehow come up with the idea that it would be ok if you put them together to make the filename. Don't fall down that trap.
I have seen people choose to put the designer's name in the file name. That's useless, in my opinion.
Really, the file name is not for the user at all. The file name is for the OS and the software that is using the file. Especially with SolidWorks, you have the ability to use custom property information which helps you identify the associated text-based, non-geometric data that goes with each document (part, assembly, drawing). Stuff like "description", "material", "finish", "vendor", "process", "make or buy", etc. is all information that needs to be associated with the part, but should not be part of the file name.
Why does the government know you by your SSN#? It's exactly the same answer. The database is keyed on a uniquely identifiable number, specifically because there may be 1000 other people in the country with your exact name.
My opinion is that the file name needs to be something uniquely identifiable, and the best way to do this is to use some sort of sequential component to the file name. It is ok to use a bit of a prefix or a suffix to briefly identify the function of the document, but this should be minimal. Something like XX-12345 where XX denotes some function (part drawing, assy drawing, model, work instructions, schematic, test results, etc), and 12345 is sequential.
Of course whatever you select needs to work for both your PDM and MRP systems, so you might want to consult the business types to see what will work for them.
The reason I said with a PDM system sequential PNs are almost essential is that the only way for PDM to identify a documet is by the file name. If you have 2 docs with the same file name, PDMWorks sees the second one as a revision of the first.
This is a frequent discussion on this ng and it is something that old- timers in particular tend to get almost religious about. Just remember that you need to have a rational reason for picking a system, and a rational reason isn't "that's the way we've always done it", or "back in the War, we did it this way", or "that's the only thing I know so it must be right".
matt
snipped-for-privacy@yahoo.com (skrug) wrote in wrote in message

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Hi Monkey -
Your problem is common for composite assemblies.
For a given component, I personally like the base number plus descriptor:
For Example 12345_Rib.sldprt, 12345_Gusset.sldprt, 12345_Bearing.sldprt going into 12345.sldasm. This works great for a composite assembly and does not needlessly "consume" numbers. My real criteria for naming is this "will this model have a unique identity in MRP or will it be 'masked' by the assembly or part it lives in?" (generally vendor supplied or parts not visible to MRP like weldment raw stock). If the part will not have an MRP record of its own, then it serves the parent part (12345) and gets an appended name like 12345_Thing.sldprt. If the part (or sub part) gets an MRP record, use that for the name.
Personally, I think it is self-defeating to "rename stuff later", it's a pain in the keester and better to have a number scheme while starting out. This is particularly true with PDM, especially when your system requires unique names. Your company has a number system which pretty much dictates what you need to use, so let that guide you.
Keep the number of BOM levels sensible if you can control it - Flat line BOMs are great, 72 tiers in a BOM are not (subs in subs in subs in subs).
Dissolving makes no sense to me as the mates invariably do not migrate upward with the dissolved components. Start where you want to end up. Think about the assembly structure prior to your modeling and try to get it structured right out of the gates.
Personally, I thing that one would like to build parity between your MRP & PDM database wherever it naturally exists. The question you pose is essentially that. MRP generally must drive CAD and one will serve the other, usually MRP will dominated as this is what is built/ordered/planned to.
This is a long ramble, but generally since the two systems MRP & PDM are not always synchronous, they can help and compliment each other while one must be the "master" the other must conform. Personally I try to make parity when possible, but if I can't I don't sweat it. Treat your available part numbers like gold and use them for something you will plan & fabricate (mrp-wise) but dont feel like you need to hijack them to manage your cad data. That always makes one miserable in the end. As you said "It may not be clear to future generations . . ."
Regards-
SMA
"Philosophy - The Science Of A Better Question"
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You could make the frame as a weldment BUT make sure that the legs are a pattern (i.e do one leg and pattern it - you could always use a sketch driven pattern). Then you only have to mate one set of your assembly components to one leg and use a 'FEATURE DRIVEN' PATTERN to populate the other 7 sets of assembly parts.
Merry :-)

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