What's new
What's new

Questions about tolerances on lathe work +/- .00025

PrawnConnery

Plastic
Joined
Jun 10, 2007
Location
Houston
I've recently had trouble making my time on a job that had a few tolerances of +/- .00025 on diameters.

The customer said he wanted to pay 22 dollars a piece for each part. It took a considerable while longer than that.

When you have a fairly short run of parts(20 or so) how do you approach these type of tolerances? OD and ID.

Material was 316ss and roughly 1 inch diameters.
 
For $22? I'd politely ask him to find someone else to do them.
I probably wouldn't be so polite.
And another thing, if we all charged what the customer wanted to pay we would all be bankrupt inside a month. You tell the customer how much the job will cost, and if he does not like it he will go somewhere else, probably to someone like the OP
 
Once tolerances drop below +/- .001" the price goes WAY up.

If it's got to be that close, you better be willing to pay for it.
 
Last edited:
Does your machine have the capability of holding that tolerance? I've run parts of 316L stainless with tolerances of +/- .0001" before, but it was on a brandy-new Star SR20-RIII. That tolerance was actually very easy to hold, once I had determined the tool life expectancy.

What machine are you using? What insert size, chipbreaker and grade? What speed (surface feet per minute) and feed rate?

BTW, these were parts about .160" diameter x .280" long, made from 3/16" bar stock and sold for under $.70 each. 17 second cycle time including spotting and drilling a hole through.
 
May be a stupid question, but what do you guys do to measure features that small. I am very fond of my gauge pin set, but they are in 1 thou increments. Do you buy a set of deltronic pins or similar? Maybe just CMM, but CMM requires the part off of the machine. Please share your secrets. Could you make a set of GO NO-GO gauges using high quality micrometers? I guess I would have to buy something better then my chinese Shars mics. ;)
I have similar situations with money and customers, but am scared to run anyone off in this finicky economy. I wonder how one goes about learning how much he can/should charge for a job.
 
I turn to the max condition, and polish them into spec. PITA, yes, but some of them come out right on, and some need the polish. 0.0002 comes off pretty quick, more than that, takes some work. If the lathe cannot hold within 0.0005, I'd be tempted to give up, or get a better lathe :D
 
Once tolerances drop below +/- .001" the price goes WAY up.

If it's got to be that close, you better be willing to pay for it.


I couldn't agree more! A broom stick handle cost so much, but a precision broom stick handle is another matter.:nutter:
 
...
I have similar situations with money and customers, but am scared to run anyone off in this finicky economy. ...

That's a formula for slavery. You've got to be constantly thinking if you are using your own limited time resources efficiently. This means getting on the phone and selling your time rather than slaving over pay-nothing jobs. Now this can vary depending on the customer. If a very profitable customer needs a favor thats one thing, but don't fall into the trap of giving away jobs to get new customers. It never works out because it sets low expectations.

...I wonder how one goes about learning how much he can/should charge for a job....
The job needs to pay for your time, your expenses and your tooling. The first, your time, only you can decide what that's worth. The second, your expenses, you need to know your burn rate. The last, your tooling, many customers assume that since you have all that tooling laying around that its free to use on their job. Don't fall into that trap. The job should leave your tool crib in better shape than when you started.

If the jobs you are bidding on do not allow you to make a decent cost recovery plus something like a living wage then you go out and find better customers.
 
Does your machine have the capability of holding that tolerance? I've run parts of 316L stainless with tolerances of +/- .0001" before, but it was on a brandy-new Star SR20-RIII. That tolerance was actually very easy to hold, once I had determined the tool life expectancy.

What machine are you using? What insert size, chipbreaker and grade? What speed (surface feet per minute) and feed rate?

BTW, these were parts about .160" diameter x .280" long, made from 3/16" bar stock and sold for under $.70 each. 17 second cycle time including spotting and drilling a hole through.

Star SV32JII turning a 7.475" long part from 1.125" diameter 4340ESR down to .632" with a few grooves and flanges in the center. Parts took over a half hour each, required manually removing the part out of the sub and closing the thread rolls. Hassle and a half, but it held tenths all day long!
 
Holding +-.0002 is a cake with the right machine and right care taken. You need both. Give a poor or misinformed programmer a half million dollar Mori and still may not be able to hold +-.001. Here are some tips. Some are obvious, some are not.

Keep tool load consistent and low. Make sure you have a rougher and finisher for every critical detail.

Move your machine the least possible. Try to move the turret the least possible between indexes. Keep useless moves down to a minimum. Optimize the best you can. I see many programmers lazy to check what clearances they have to they just program the machine to home before making an index. This makes the ballscrews warm up more than if optimized.

Slow down your rapids. Sometimes it helps.

If using a barfeeder be aware that as your bar gets shorter some dimensions will change. Less weight on your spindle. Also bar whip and vibration will need to be kept to a minimum.

Many times I dont bother running a warm up program. Just run the part program without a part in the chuck. Loop it with an M99. Let it run for 30 minutes or an hour. Then you can make some parts and do some fine adjustments. Try to keep the machine running while in the groove. Eat your lunch next to the machine.

Have at least 40 gallons of pre made coolant sitting next to the machine at least 8 hours in advance. Nothing worse that putting 20 gallons of 60 deg coolant in a machine that is 90 deg.

On fine tolerance features turn of G96 and stay on G97 ( constant rpms).
Always changing rpms not only disturbs the spindle location ( yes it does) but also makes the amperage draw on your machine inconsistent and traces into your servo drive and may affect encoder feedback and accuracy. Not all the time, but sometimes. It is better just to eliminate this possibility and use G97.

Leave your machine on all the time. Once your hydraulic oil and sump get up to temp. Dont let it cool by shutting off the machine.
 
22 bucks might not be that bad depending on the part. Do we even know what these parts look like?

Also, that tolerance is a total of .0005. That's not really so hard, is it? I know it's not like .001 but geeze, I've worked in shops that had to hold this nearly on a daily basis.
 
22 bucks might not be that bad depending on the part. Do we even know what these parts look like?

Also, that tolerance is a total of .0005. That's not really so hard, is it? I know it's not like .001 but geeze, I've worked in shops that had to hold this nearly on a daily basis.

Yeah, it doesn't sound too bad (with the right machine, etc...- what the other posters have been saying). BUT with a quantity of 20? Maybe I'm not that good but it takes me a while to dial in those kind of tolerances.
Price was too low for those quantities IMO.

Frank- great listing of things to watch out for.
 
Yeah, it doesn't sound too bad (with the right machine, etc...- what the other posters have been saying). BUT with a quantity of 20? Maybe I'm not that good but it takes me a while to dial in those kind of tolerances.
Price was too low for those quantities IMO.

Frank- great listing of things to watch out for.

I understand what you're saying. It does seem too low for most parts. That tolerance on 316 stainless, is a little different than that tolerance on brass.

But, for all we know, this could be just a bushing.:confused: Probably not though.
 
Most modern machines would hold that tolerance, fairly easily. The biggest problem is that most shops aren't set up to _measure_ that tolerance properly.
If you can't measure it repeatably, you can't machine it repeatably, even though the machine can do it.
You start chasing your tail over what you think are machine problems, material problems, tooling problems, etc when, in actuality, it's a measuring problem. Most folks in the job shop trade I know don't have a good grasp of this.
When you get proper measuring equipment for that tolerance, it becomes much easier to machine it.
For that tolerance, you need measuring equipment accurate to 0.00002. (10x more accurate than your tolerance.)
One of the issues with the job shop industry I see is they will buy the best equipment they can afford, but still use vernier calipers and an 0-1 (0.001) mic to do the measuring with. The machine will hold 0.0002 all day, but they can only measure repeatably to 0.010 with the equipment they have....
 
If you have a tolerance of .0005, you can easily read an od measurment with a mic, and for I.D. it's easily seen with a bore gage.
 
I hold .0005 total tolerance on bores all the time on lathes - most of our work is exactly that; a bore that's roughly 4-5x diameters long, and the diameter is +.0005/-.0000. Part runs anywhere from 20 parts to 400.

Set a tenth reading bore gauge. Job done. There really isn't anything to it, you just have to check each part and get an idea of where the machine is going to be on the next part.

The first part should come out right; sneaking up on a bore is a simple matter. Each time you take a pass on your setup part where you've changed the diameter, you need to make a skim pass before you change the diameter again. Sneaking up on stainless is relatively easy; it's aluminum that's difficult.

So you have your first part, but the next part is still going to come out wrong. Note how far out it is, -.0007 or something. Write it down. Now sneak up on the diameter again. It'll take less than .0007 to get there; after you've finished sneaking up, add enough offset to make up the .0007 measurement. Say it was .0007" out, but between spring passes and adjusting offsets, you only needed to move the machine .0004". Move it another .0003" - the next part should be dead on.

Also, in the morning, I don't bother warming machines up. I note where the machine was, size wise, the last part of the day. Next morning, I bump the offset down .001-.002. Run the part. It'll be a little bigger or smaller; I write this number down, and every morning thereafter all I have to do is enter the difference between the expected and actual I got that first day. I figure I have to babysit the machine anyway, so might as well not waste time warming things up.
 








 
Back
Top