Finally wrote-up my "How to Design Parts" section...

A few comments are in order.

I looked at the first drawing. There is likely a big problem with it although machinists will love it. Note that the location of the two through holes is off the back edge of the top view. In fact the left rear corner of the part is the origin for all the dimensions. While this makes it easy for the guy on the Bridgeport to setup the job the all important tolerance stackup on the part has flown out the window. More than likely the spacing between the two through holes will be critical to fitting a mating part. Yet there is +/- .010 on the spacing even though three place tolerance is +/-.005.

Second, the drawing specifies a pocket. This is a manufacturing term for a specific process. I couldn't tell you what pocket means from my GD&T book in the same way I could a hole.

Rule No. 1. The drawing should define a part without specifying manufacturing methods.

Finally, there is a double dimension on the part. In the top view .250 deep pocket is stated. In the front view a hidden line is dimensioned .250. One of these should be a reference dimension.

Rule No. 2 Dimensions should be arranged to provide required information for optimal readability. Dimensions should be shown in the true profile views and refer to visible outlines.

This part is a good case for a section view or at least a removed section to make the hidden bottom edge of the "pocket" visible to dimension off of.

And of course it is common practice to place as the front view the view with the fewest hidden lines. I looked at your web site and you are in the USA so you would probably be using 3rd angle projection for your customers.

Thank you for this document. It will be very useful to pass on to my office. You wrote down a lot of information that was previously word of mouth in a clear fashion.

Thanks for the comments. Yes, there are a few faults in the print. This was not meant to be a "perfect" print as per CAD style guidelines (you can write that e-booklet yourself :-)). The point was to show a real-world print that would yield a decent part without confusing the machinist and wasting time and money. Truth is, we *very rarely* even see prints this good!

In regards to your point, I did think about the double dimension, but liked the clarity of it. I should add a "ref." though, you are right. A sectional view was hard to fit on this A size paper. The hole spacing is a good point, but these are threaded holes, for goodness sake, not precision alignment pins. There are nice sloppy screw clearance holes that mate with them, .010 is just fine.

Thanks for the feedback though, I do really appreciate it.

Joe O.

Thank you for the kind words parel. I appreciate them.

Best Regards,

Joe O.

hey thanks for the thought and time you put into this. you couldn't make a pdf of it? could you please :o)

Hi Neil:

I'd be happy to do that if I knew how. Is there some common (free) software program I can use? I don't have any adobe programs on my machine.

Joe

With 3D CAD the section view or removed section would be a piece of cake and take up no more room on the sheet. Probably the clearest representation of the part would be with an offset section in place of the top view assuming you made the current top view the front view per commonly accepted practice.

OK, Ok, I give up. I've revised the print. Have a look now and see if you like it better ;-).

Joe

Joe,

I always appreciate working with a machine shop that is willing to listen to a customer. :)

TOP

P.S. The guy assembling this will love you for it too.

In my case, I work for the machine shop, and I agree with Joe on the specific case of the tapped holes. For one-off or short runs, our guys prefer to have everything come from the same edge, even if I have to tighten the tolerance to do it. Within limits, of course. For a tapped hole though, a .005 tolerance is not significantly more difficult or time consuming than .010 tolerance. Our inspection department also prefers that I use fewer datums, because it's less work for them also.

As we use more and more automated machining and inspection programming from the models, I'll be able to relax on all that and start using more model dims. Until then we prefer to have fewer datums, and customers who supply designs with a lot of datums and setup will have to pay more because it takes significant time. Better drawings means cheaper parts, quicker.

Regarding your tip about using "yellow dimensions" on a white background: I just had some experience with this nightmare. A potentetial client had over

100 C sized AutoCAD drawings (with yellow dimensions) that he printed out on letter sized paper. They no longer existed in digital form. He wanted them translated into SolidWorks-parts, sub-assembly, assembly, and drawings. Needless to say, I turned it down. I could hardly even read the things with one of those large inspection magnifying glasses.

Mike

Good stuff Dale. Thanks for writing. What you say is right on the mark. This particular part (which by the way doesn't really exist, I made it up for the example) is pretty simple, so it is not a big deal either way. But fewer datums makes a big difference with fancier parts.

Thanks again for the note.

Joe O.

Best Regards,

Joe

What is it about AutoCad that makes all these yellow dimensions? Was it a common default color? Or something in translating .dwg or .dxf files? Amazing how often you still see them.

Thanks much for the great story and comments!

Joe O.

Just lazy operators who couldn't be bothered to setup plotstyle table and map colours to black.

Mostly good. This from someone who was a machinist. Definitely good reading. A sound study in "design for machinability".

Definitely agree about colors. Prints should make sense in black and white (not even greyscale).

Definitely pay bills on time! I take care of my vendors, including the occasional trip to purchasing to make sure the little guys get their well-deserved and much-needed cash flow.

Contact name on print? No way. Does not belong on an engineering print. Should be part of quote package, but not on print. My people are not going to do an ECN every time project responsibility is shifted.

Don't like to quote? There are more direct ways to terminate a business relationship, but that one will work fine. However, it is in everyone's best interest to have a well-crafted quote request. Ask for what you want, because you'll probably get what you asked for.

Great stuff--well written.

I can help with the PDF if needed--I'll save as one & send to you if you'd like. Just let me know.

If you'd prefer to save yourself, try PDF995

free) or PdfFactory trial).

Thanks,

Brian

Yeah, they're using the default black background. Yellow and cyan look great on a black screen. Too bad they're not printing on black paper.

Mike

Dale,

I've been down this road before. Here is the problem. Every machine shop has their preferences that usually depend on the background of the machinist(s) and the equipment being used. And of course the inspection department is going to want to minimize their work. So it is possible to make a print that one machine shop likes and another doesn't. This brings me to the ANSI specification and the engineering side of things. ANSI makes a big point that a print is not to specify manufacturing methods. The engineering side is concerned with form, fit and function. The part should be dimensioned primarily so that if it meets the dimensions specified it works first time and every time. If you can use Joe's methods and still assemble the parts after doing a tolerance stackup then I agree that that method is going to be the least expensive. Bottom line though is that engineering shouldn't be second guessing manufacturing. And the machinist shouldn't be concerned with the fit of parts, but rather making parts that meet print.

Now as far as tightening tolerances to be able to work off one edge I have a little story. One place I worked would throw a .0005 tolerance on in cases were working off one edge made the tolerance stack not work. Then they would throw the part out for bid and take the cheapest shop. What usually then happened is that the cheapest shop couldn't hold .0005 if their life depended on it.

I think what you really want is to have working drawings for the machine shop that may be dimensioned differently from the drawings the part should be inspected to. This makes it easy for the machinist to setup.

It can be a difficult balance. While I don't specify how to make a part, I can't ignore what it takes to make a part. As you mentioned, different shops will have different preferences according to experience and equipment. Being aware of what a shop can do, a drawing can be tailored to those capabilites. Also, candidate shops' capabilites should be matched to the parts they are working on.

I don't see ANSI drawing spec entering into the discussion. We're not talking about specifying which tools the shop has to use to create the required geometry. We're talking about being aware of what a shop's needs and capabilities typically are, and taking advantage of them.

Your unfortunate experience with the lowest bidder seems to me to be an example of why price should definitely NOT be the only criteria for who gets a job. If the shop bid on a job that they couldn't do, then their price is not a useful measure of the most cost effective way to organize a drawing. That is, they failed to correctly evaluate the job. The data should be thrown out. In the specific case of holding .0005", that may be a case where a setup is actually added to the machining, because the machine that taps holes probably can't reliably place holes to .0005. So the part will have to be set up on another machine that can handle that job.

I thought for a bit about your suggestion that what I actually want is a separate drawing for machining and inspection. Maybe that's not what you actually meant, but I don't see how that would help anything, and I didn't mean to suggest it at all. Why would I want that? Machinists know that a part will be inspected to the tolerances they see on the drawing, so they make sure it's right before they're done with it. I don't see any purpose in disconnecting that. I must not be clear on what your trying to say there.

One might argue that tolerancing should be derived solely from fit and function, and that reference dimensions can facilitate simpler setups. I think this is reasonable, but it makes more work for everybody. The drafter has to add the extra dimensions, and the machinist has to reinterpret the tolerances for his setup to be sure that his part will pass inspection. Everyone I know is happier when I give them toleranced dimensions they can work to and the part will fit and function. They are free to make the part however they want, but I try to make it as simple as possible.

I don't think this is unique to our shop, or simply a preference of a few stubborn machinists. We have a lot of guys from a lot of different backgrounds, and I get similar feedback from all of them on what makes their life easier.