Working Drawings

[ddmathias]

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.

 

[maxh3]

We're fairly small and I've pretty much made all decisions pertaining to part drawings, but I'll tell you what we do (and I try to keep sheets A sized since we don't have a plotter yet.)

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.

 

[maxh3]

I also try to keep sheets "A" sized since I know many of the machine shops we use don't have a plotter, and can only handle printing 8.5" x 11" sheets, though sometimes on a larger part I'll have to bump up to a "B" which isn't terrible looking when printed scaled down on 8.5x11.

BTW, is there no way to edit posts on this forum?

 

[CADFlyer]

This is the way our company handles it.

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.

 

[SnowCrash]

Often I will create a part drawing with dimensions and another file with the image of the CAM paths and data on the machine setup.
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

 

[tristram]

My 2 cents.
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

 

[CorBlimeyLimey]

You will probably get several conflicting answers because many companies have their own standards.

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.

 

[gwubs]

I agree with your husband. Here's why: you can reuse those parts over and over. That part drawing tells how to make the part, the assembly says how many, and where to put them. No missing, or duplicate info that way. Use assemblies as sub asseblies, and presto - it calls up all the part drawings. Seems like more work, but it's clean, organised, and reuseable. And it is this reuseability that many companies do not achieve, and as a result never go as fast as they did before (in flat cad).

 

[drawoh]

ddmathias,

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).

JHG

 

[SnowCrash]

Maxh3,
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

 

[DiegoLGraves]

dd, welcome to SW. I use separate drawing files for parts and assemblies. This helps with file sharing for sub-contract work. And in our business which is primarily sub-contract fabrication, I prefer it when customers send individual prints for components. Revision control is easier, or at least seems easier. Also, at least before we bought new spectacular workstations last year, SW multiple page drawing files could bog down the computer.

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

 

[ctopher]

I agree with your husband.
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

 

[jassco]

Hi, ddmathias:

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,

 

[hititfaster]

I work for a bureau, so we have lots of clients with LOTS of ideas of what is right/wrong and I have to work with all of them in several different CAD packages!

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!

 

[ewh]

I agree with your husband.
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." - [small]Robert Hunter[/small]

 

[ddmathias]

Thanks to all for your replies. I'll go forward with this so my students don't have any rude surprises in the real world.

ewh: How can I get a copy of the ASME standards you referred to?

 

[ArtL]

ddmathias The ANSI / ASME standards are in the "Machinery's Handbook". Also called the machinist "Bible". You can get it as a book or CD.

 

[ewh]

Global also publishes a small Drafting manual that follows the standards, probably less expensive than the Machinery's Handbook, definitely less expensive than the actual standards.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[fcsuper]

You may wish to read ASME Y14.24 - 1999 which covers types and applications for various types of Engineering drawings. Generally, the only time I would make a single drawing for an assembly is if it is an inseparable assembly.

Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
Follow me on Twitter

 

[MikeHalloran]

One outfit I worked for no longer uses assembly drawings at all in the usual sense. No doubt they're produced internally for engineering purposes, but they're not officially issued or maintained.

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