Working Drawings
Working Drawings
(OP)
I am a college instructor who has just started teaching SolidWorks. I have taught AutoCAD for many years, and have instructed my students how to lay out and assemble a set of "working drawings" per the various graphics textbooks I have used over the years. My husband, from the manufacturing industry, disagrees on how a set of drawings should be laid out, based on his industry experience. I'd like some feedback from others on what current practices are. My definition of Working Drawings is a set of drawings that includes an assembly drawing and the drawings of all components, so that the entire assembly can be manufactured and assembled.
My idea of this is to have a set of sheets, with one or more drawings on each sheet. So, we could have drawings for 2 or more parts on one sheet. Each part drawing would have dimensions and a note associated with it giving the BOM item number in a balloon (but without the leader since it is a caption), part name, material, and quantity required. The assembly drawing would have a BOM, balloons, and other assembly information. The detail drawings and assembly drawing are all part of one sheet set and are numbered "Sheet 1 of 4," etc, with the assembly drawing on the last sheet. This was all easy when drawings were hand-drawn, but seems awkward in SolidWorks. For example, I haven't yet figured out a way to create a ballon with an (automatically generated) item number in it and no leader.
My husband's idea is different, and is much easier to produce with SolidWorks. He says that each part should have its own paper, as should the assembly. No material on the assembly drawing. No captions on the part drawings. No sheet numbers (1 of 4, etc.).
Any comments? Is there a published minimum standard? I realize that all businesses will have their own drawing standards, but I'd like to get a feel on general industry preferences. I'd like to teach my students something that they are likely to see when they start working.
My idea of this is to have a set of sheets, with one or more drawings on each sheet. So, we could have drawings for 2 or more parts on one sheet. Each part drawing would have dimensions and a note associated with it giving the BOM item number in a balloon (but without the leader since it is a caption), part name, material, and quantity required. The assembly drawing would have a BOM, balloons, and other assembly information. The detail drawings and assembly drawing are all part of one sheet set and are numbered "Sheet 1 of 4," etc, with the assembly drawing on the last sheet. This was all easy when drawings were hand-drawn, but seems awkward in SolidWorks. For example, I haven't yet figured out a way to create a ballon with an (automatically generated) item number in it and no leader.
My husband's idea is different, and is much easier to produce with SolidWorks. He says that each part should have its own paper, as should the assembly. No material on the assembly drawing. No captions on the part drawings. No sheet numbers (1 of 4, etc.).
Any comments? Is there a published minimum standard? I realize that all businesses will have their own drawing standards, but I'd like to get a feel on general industry preferences. I'd like to teach my students something that they are likely to see when they start working.






RE: Working Drawings
If the assembly is small/simple, such as a part with some dowel pins pressed in, or a couple of parts bolted together, and we expect one supplier to manufacture and assemble completely for us, I'll generate a single drawing file with multiple sheets. The first sheet will include a BOM and a view or two of the assembly, one of them ballooned. The assembly will have its own part #, and each part will have its own part # as well, something derivative of the assembly PN if it's a custom part for that assy (not a screw, etc.) Each part drawing will be on a sheet following the first assembly sheet (unless it's an off-the-shelf part, then no drawing.)
If it is a large assembly, the assembly drawing will be its own file, perhaps with multiple sheets including different views, an exploded view, BOM, assembly instructions, etc. Then each part will have its own drawing file with one or more sheets depending on how complicated and how many views I need to include.
BTW, to remove the leader on a ballon, click on the balloon to highlight it and activate the property manager toolbar, click on "More Properties..." at the bottom, look for the "Leader" section (you may have to expand it) and there will be a button showing a leader with a red X by it. Click that.
RE: Working Drawings
BTW, is there no way to edit posts on this forum?
RE: Working Drawings
Each part and/or assembly has it own electronic drawing file.
A part/assembly file may have more than one sheet(shown as tabs) depending on paper size that is pre-defined.
I have found that it is much easier to match 1 model to 1 file for file management reasons.
Solidworks offers both on-line & in-class training on file management.
RE: Working Drawings
The part numbers and assembly numbers and drawing numbers are similar, but the drawing number includes the date code when last revised.
Data on the drawing is just enough to make and inspect the part.
--
Hardie "Crashj" Johnson
SW 2011 SP 2.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580
RE: Working Drawings
I agree with your husbands way of doing things.
Every company has their own way of documenting and working with their drawings/data. I think the main reason your way of doing working drawing is out dates because it is not very PDM friendly.
You also run into a problem if you want to use a part on/in a new assembly, you will have lots of duplication of information in your system. Or if some one needs a replacement part they have to pull a 10 sheet drawing and look for the parts detail sheet.
I have worked for many companies as a contractor for many years and seen many systems and believe the best system (and what I use in my company) is a non-smart part numbering system and every part gets it's own drawing, even purchased parts.
-Joe
SolidWorks 2009 x64 SP 5.1 on Windows XP x64
8 GB RAM - Nvidia Quadro FX1700
RE: Working Drawings
I'm inclined to agree with your husband, but it's usually a company choice whether to use single-sheet or multi-sheet drawings. Each have their pro's and con's.
Either way, the assy's are the "index" to the parts, and as such should be the first sheets in a multi-sheet drawing. The item (balloon) number is just a simple reference to a line item in the BOM ... it does not need to be added to each part drawing ... the part drawing number should suffice.
Generally, part numbers and sheet numbers match.
RE: Working Drawings
RE: Working Drawings
I agree strongly with your husband. If drawing 123-456 contains three components and I need to modify one of them, I expose the other two components to modification. At the very least, I need to convince my fabricator that we modified part 123-456-02, and not 123-456-01 or 123-456-03.
If you are building one-offs, this is much less critical. Multiple parts per drawing might save some time.
In manufacturing, you must consider the total lifespan cost of the drawing(s) and part(s).
RE: Working Drawings
Incidentally, on format size, I use B size formats and print on A size paper, scaling the drawing to fit. This leaves a margin at the top and the hole punches there do not cut out any part of the drawing.
As far as multiple sheets, I have found a good use is when I have a vendor do part of the machining and bring the piece in house to be finished. The vendor gets sheet1 with the mods suppressed, the shop gets sheet2 with a config with the added features.
--
Hardie "Crashj" Johnson
SW 2011 SP 2.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580
RE: Working Drawings
The only regular exceptions now in making multiple page drawings including assemblies and parts are for conceptual designs, made before individual component parts are made, and fixtures for our shop or for our vendors or customers.
Diego
RE: Working Drawings
All parts have their own drawings, with revisions.
The sub-assemblies and final assemblies how their own drawings with BOMs or PLs.
Model and draw them as they are made.
Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion
RE: Working Drawings
Your husband is light years ahead of you in regard to document management. Because of database nature of 3D modelling, it is best to document each item with its unique document.
One part model (*.sldprt) per item with a drawing document (*.slddrw) if necessary.
One assembly model (*.sldasm) per assembly with an assembly drawing document (*.slddrw).
Since you teach SW at college, you may want to get yourself fimiliar with PDM and revision control.
Best regards,
RE: Working Drawings
By an English mile I prefer working in SW. Personally, I'm with your hubby on set-up and so is our biggest client, so that's what I prefer. My boss drums into me the following:
1. One part per drawing. Part numbers are the most important thing describing the part and the drg. number IS the part number. IDing is easy and so is calling up replacements should they be needed.
2. Sub-assemblies: produce an assembly drawing then subsequent part drawings. Use the part drawings to make all the parts and then the ass'y to assemble all the pieces. Fixings go in the ass'y drg. with a BOM.
3. Full build is done in a top-level GA drg. This is where you bring together all of your parts and sub-assemblies, again with a BOM showing fixings.
There are some exceptions to the rule, but these have been few and far between. Pretty much I agree with everything you've all said re. this method. I was skeptical initially, but now any other way of doing things seems awkward!
RE: Working Drawings
As far as minimum published standards, the vast majority of manufacturing companies I haved worked with follow the ASME (previously ANSI) standards, with exceptions or additions noted in company drafting manuals.
"Good to know you got shoes to wear when you find the floor." - Robert Hunter
RE: Working Drawings
ewh: How can I get a copy of the ASME standards you referred to?
RE: Working Drawings
RE: Working Drawings
"Good to know you got shoes to wear when you find the floor." - Robert Hunter
RE: Working Drawings
Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
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RE: Working Drawings
BOMs are maintained only in their MRP system, and printed as needed.
Engineering produces and maintains only component drawings and specification/source control drawings. Every part gets a document and a number.
They don't make, stock, handle, number, or document subassemblies.
Manufacturing/assembly instructions are documented a few steps at a time, a few A size sheets per JIT station, showing in excruciating detail, pictorially, what is to be done and how. Those documents are maintained by Manufacturing Engineering, who treat the marked up prints at the workstations as the masters, and try to keep up with computerized versions later.
It was a nightmare to set up and get running, but it works pretty well.
The original manufacturing instructions were produced by a team of artists, who chose not to use the CAD documents that were available.
I have no idea how effective Solidworks would be in that environment. It should be possible to use it to produce the artwork for the manufacturing instructions, but it may or may not be faster than an artist.
Maybe somebody is using SW for JIT somewhere?
Mike Halloran
Pembroke Pines, FL, USA
RE: Working Drawings
As far as I am concerned, DFMA rule number 1 is to prepare assembly drawings. Once you have prepared assembly drawings, you can show everyone that you have thought through the assembly process. If my responsibility does not extend past a stack of fabrication drawings, the assembly process could be very bad.
Imagine you are writing instructions on how to change spark plugs on a pickup truck. If you are a technical writer, you explain how to open the hood, place the truck on a hoist, lift it, remove the front suspension and the engine bolts, lower the truck and lift the engine, using a winch. If you are the designer, you make the spark plugs accessible, and write instructions on how the spark plugs are visible and accessible when you open the hood.
It ought to be possible to set up a web page with JPEG views taken from the SolidWorks model. You would need to find some way to verify what revision of your model was used to create the JPEGS.
RE: Working Drawings