17 Tips for Designing Cost Effective Machined Parts 11

[haileyk]

FYI, we just published an article from a thread of discussion at Eng-Tips Forums at ENGINEERING.com. Hope you enjoy it.

17 Tips for Designing Cost Effective Machined Parts

 

[Jboggs]

Thank you haileyk and ctopher! A very good article. Even after 40 years of doing this I learned a few things. I'm one of those guys who has spent his life designing components to be made in a machine shop, but has no direct machine shop experience. I have always tried to treat my shops professionally and with respect. I frequently ask for their advice on how best to achieve my design purpose. I try to make sure my drawings are clear, thorough, and as simple as possible. I have found that if I treat them with respect they will return it in kind.

 

[Sparweb]

Excellent advice. Thank you

STF

 

[arunmrao]

Thanks for the excellent tips. I have shared them in my machine shop.


"Even,if you are a minority of one, truth is the truth."

Mahatma Gandhi.

 

[tbuelna]

One field that I have always felt to be greatly under-appreciated is manufacturing/production engineering. Design input from a good manufacturing engineer can significantly reduce unit cost, improve quality, lower scrap rates, and increase production rates. Sometimes the most effective way to reduce cost is by using a raw material form (such as a casting, stamping or forging) that needs less final machining.

One of the most impressive examples of mass production engineering I can think of is the stamped steel rocker arm used on millions of GM OHV engines. It was invented by a manufacturing engineer at Pontiac named Clayton Leach. The management at Pontiac did not think Leach's idea was worth pursuing at the time, so Leach worked to perfect it in his own garage, with his own money. His simple stamped steel rocker arm design likely resulted in many $millions of profit for GM over the years.

 

[Nereth1]

This has probably been discussed to death in the past, but the only thing I don't agree with is "...always dimension from the same point to avoid tolerance buildup.". Best practice in my book is to dimension to and between the things that you want to control. For example if I have a precisely sized mating slot somewhere on a long surface, but I don't care where that slot is, then if I dimension both sides of it to a seperate datum line on the far end of that surface, then both sides need a very tight tolerance over a long distance to that datum line.

If I just dimension what matters, then I will have a rough dimension to one side of the slot, and a very fine dimension across the slot. One less accurate dimension to make, and it's a much easier one because it's that accuracy over a shorter distance, and it can have twice the tolerance size because the error to the datum in one side of the slot no longer makes a difference.

The only issue with this philosophy in tolerancing, that I have run into before, is sometimes, the tolerance scheme that leads to the theoretically easiest part to machine from a machine capability point of view, ends up being very unclear to the machinist. And if the tolerances are all quite easy to achieve anyway, it doesn't add much value, especially for short runs where programming is a large part of part cost.

 

[emorrison]

"8. Avoid designing parts that have corners the same size as a typical end mill diameter. Adding .20 or .30 to any corner with a standard diameter will lessen the surface area coming into contact with the part."

As an engineer who spent most of his former life in my father's mold shop making parts, I'm more concerned with the aspect ratio of the cut than the chosen corner radius.

In other words, the component's internal corner radius and the height of that wall dictate the tool diameter required to achieve a favorable arc of engagement. What you really want to understand at that point is... whether or not standard tooling (length/diameter) can create it or if the design necessitates a more costly solution. Most likely... the more costly machining solution could be avoided all together if we follow tbuelna's advice and do a little consultation.

But if you're designing machined components, you should have some basic understanding of the standard/off-the-shelf tooling your shop employs.

 

[JNieman]

Odd-ball sized corner radii, while having good intentions, can sometimes be unnecessary and confusing. If you simply throw a "4x R 1/4" dim on a corner, and your fractional tolerance is +/- 1/8, they're free to take their 1/2" cutter and swing it around a 5/16 radius and be in tolerance, if they must. Otherwise, a lot of times it's more efficient just to drill all the corners and completely eliminate the 'corner wrapping' as the mill goes around.

The flip side to designing-for-manufacturing is that you can sometimes take it too far and make solutions to problems that don't exist. You really have to have a good foundation in the particular manufacturing process to be able to make wise decisions. More preferable to the 'oddball radius size' for non-critical features, in my opinion, is to simply specify the maximum allowable radius, or a min-max radius range, if you don't want the corners too-tight, depending on application. That'll give us much leeway as possible.

Overall it's a really good point that will make green designers put themselves in the manufacturer's shoes, so it's a good tip overall. Just felt like adding another layer to the onion, I suppose.

 

[KENAT]

Well JNieman, ignoring that fractional dimensions aren't supported by current ASME drawing standards...

From a tolerancing point of view I agree with your idea of loose tolerances on <edit> internal <edit> corner radii to give the machine shop flexibility. For corners where the radii can't functionally be too small (usually stress concerns drive min internal radii on parts I've designed) then I'll often use what appears to be an appropriate nominal tool radius (allowing for 5X max cut depth rule of thumb or similar) then add .02 to .03 and make that the max radii.

(Can get a bit messy on models feeding into CAM depending what dimension/tolerance designation flexibility your CAD has but hey, you can't always address everything.)

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[JNieman]

Not everyone cares about ASME drawing standards...

or, as in my workplace, we see them more as "guidelines" than rules, like the Pirate Code.
edit-to-add (nor do we claim compliance with ASME standards in any completeness)

 

[ornerynorsk]

#15. Fixturing wax also works well. Adhesive tape can be a bit dodgy, and usually has a little "give".

It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

 

[KENAT]

Our vendor uses magnets on some stuff - I think mainly for extremely flat grinding.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[emorrison]

Like many engineers, I'm always looking to design-out potential problem areas. Getting back to corner radii in 'fit' type pockets, I prefer the relieved corner approach to trying to control min/max radii. (see attached)

If you design (if feasible) the corner such that even a non-radius 'male' could fit, then you've left control of the fit to the length/width of the pocket (unilateral + tolerance) vs. the length/width of the component (unilateral - tolerance) occupying it. Works really well for male components that have--or must have--really small corner radii.

Back to machining, this leaves a corner that lends itself well to high-speed machining practices, where the goal is to maintain x% tool engagement throughout the process or rest machining, where a much larger tool could rough the pocket, leaving only the undercut portion for the smaller tool. And of course, all of this is out the window if corner clearance needs to be tightly controlled... and in some work, it does.

Fit is easily checked with hard gaging, like many shops still do. If the gage fits, the component should too, with no corner radii interference issues.

 

[KENAT]

emorrison, I've considered posting all the alternative ways to machine corners of a 'socket' so that it will accept a square 'plug' - yours is one of the more elegant versions I've used.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​