Results 21 to 40 of 40
06-26-2009, 08:43 AM #21
I've done some tight stuff where it's all programmed in G1's.
No rapids at all. The machine stays a lot more constant.
06-26-2009, 10:50 AM #22
With this kind of tolerance on a lathe the first question I'd be asking is where to you want the parts measured. Top of the tool marks or bottom???
You can hit this on most newer cncs but be aware due to surface finish different gauging methods are gonna give you different readings. Of course maybe you tooling is good enough to hold a 10 or better on the Ra.
At these numbers it becomes very important to understand how the customer is going to measure the part. Once things get down to a couple of tenths I've spent way too much time educating a customer about gauging variations.
If your lathe only has a least increment of .0001 it's gonna be hard to get a decent Cpk here.
Not saying it can't be done, and there are shops that do this all day long, but this is pretty tight.
I'm sure some will jump up and down at this but you are way outside of micrometer and dial indicator measuring here. This is temp controlled LVDT and air gauge range and even getting these two to agree when it's time to make an adjustment will drive ya nuts.
With a nice machine this is more of a measuring problem than anything else.
Holding 2 tenths is not so bad, knowing where zero is can be a big problem.
My experience has been that a trip to the customer to see how they are going to check the parts saves a lot of headaches down the road.
At 22 bucks I'd think this was crazy unless the volumes were decent or it was a simple turn/bore, at something like 5 pcs I'd think you'd be in trouble. At 20pcs, maybe if you've got gauging with an R&R in the microns.(depending on who is buying material?)
Last edited by CarbideBob; 06-26-2009 at 01:00 PM.
06-26-2009, 11:58 AM #23
One of the random jobs I do that has .0005" tolerances.
Shop rate, 75 bucks an hour. My part cycle time is 6m30s. It's got a bunch of grooves that like to chatter, so that's most of the cycle time. The bore itself is quick.
My scrap rate on this job is about 5%.
$75/6.5*1.05 = $12.12 per part. So add setup, and some change, and I'd buy it for 22/part.
Why are people losing their shit over this? Am I missing something? Are the cycle times on your job ridiculous? A .0005 bore should not be spawning a thread with all kinds of ridiculous gauging and other shenanigans. Maybe it's just because I do it all the time and it's not particularly spectacular?
06-26-2009, 12:14 PM #24
Glad to see I'm not the only one feeling this way. To me, most jobs have a rougher and finisher anyway, so when you suddenly plug a .0005 tolerance to a feature, it doesn't add all that much to the price. But then again, maybe that's why I don't own my own building yet.
06-26-2009, 01:14 PM #25
Maybe I'm too naive to be worried about this. My machine only has .0001 resolution, but it'll hold that when cold or fully warmed up. Most of my tolerances are +0 -.002 or +-.005, depending on the part. When I get a +0 tolerance, I try hard to hit it on the nose, I don't program it for undersize. Like others have said, it depends on what the part looks like, so I'm not going to weigh in on the cost.
06-26-2009, 01:33 PM #26
Don't get me wrong, .0005 tolerance is nothing to sneeze at. But it's not that hard with most cnc lathes. It's all in what you're used to working with. I've had people tell me that they can hold .0002 with their lathes, and I think they're nuts. To me, that's the limit for machining, and that should be ground, but some people claim to machine it. It's all in what you're used to working with on a regular basis.
06-26-2009, 02:42 PM #27
Glad someone else piped up on this.
Tolerances under .001 total always get a semifinish pass @ .002-.003 leave allowance on the diameters using a separate tool ( not the rougher, nor the finisher!!!)
I that case there is very little wear on the finish tool, cut depth is nearly constant so you should not have to adjust the offset after the 3rd part for quite a while in any materials, including nickel or cobalt based alloys.
I'm no hero by any means, but this is quite easy and commonly done here, and the price doesn't increase too much either.
Having said that, I try not to quote anything under .0005 overall for "good stuff" materials, dims under .0003 are never quoted without honing or grinding included. For common steel parts I draw that limit @ .001 total. No exception!
06-26-2009, 04:08 PM #28
Several years ago when I was working as an applications engineer for a machine tool importer/distributor, I had a new Swiss-turn lathe set up to run a test for some 4140 steel bushings (a Harley transmission part) with +/-.00015" tolerance. From a cold start, a Cpk of 1.6 was required to qualify the machine. The program had to be under 27 seconds, so all the rapids were in there. The machine's least programmable increment was .0001".
The part run of 250 pieces was a 2.0 Cpk. So it is possible to achieve consistent high-quality results with rapid traverse moves, tight tolerances...and a new machine.
Oh, and every surface was done in a single pass. Face, drill, bore, roller burnish I.D., turn O.D., roller burnish O.D., cut off.
06-26-2009, 05:16 PM #29
On just a plain turn with only 3/10's to play with, having a machine that makes 1/10 jumps makes it interesting to decide when to adjust size.
Again, this is not that hard to do if the machine is nice and you've got control of temps but getting accurate and repeatable measurements so you know where you are is the biggest problem.
Making a handful of parts within a couple of tenths is easy.
Making them all within a couple of tenths from zero is another story. Specially when you throw taper and ovality into the numbers.
Many here are obviously doing it, I've just spent too much time building gauges, autocomp, and SPC systems so I'm overly picky about my measuring. Somewhere along the line I quit trusting any measurements.
06-26-2009, 05:55 PM #30
A cpl of you guys have said that a half thou total tol doesn't add much to your priceing. Which is fine. But does that mean that you were overcharging for .010 tol parts?
I have some parts here that have up to 4 bearing bores in one part. Tols ranged from .0005 to .001 total for whatever reason. Boring was done on the main as well as the sub to git them all. 1200 series material didn't hurt anything tho.
I was quiet impressed how well it went, but it still required babysitting. After while I just shut everything else down to babysit it and git it out the door.
For the tighter bores (to make things as easy on myself as possible) I tried to run them on the tighter side, and if one came in undersize occassionally - I would scurry it on over to the engine lathe that I had a burnish tool all prepped and ready to go. That's only good for a tenth ... MAYBE you can squeeze 2 if your S/F is rough enough. But how rough'a finish does enyone have when your going for tenths?
Think Snow Eh!
06-26-2009, 06:10 PM #31A cpl of you guys have said that a half thou total tol doesn't add much to your priceing. Which is fine. But does that mean that you were overcharging for .010 tol parts?
06-26-2009, 06:22 PM #32
06-26-2009, 06:31 PM #33
Ox, I generally have to babysit every machine I'm running no matter what. So to us, because of flow and equipment problems, it really doesn't add much in the way of cost. If I had nicer machines (like you, you bastard), and a better workflow to accompany the equipment, I'd be really hostile about having to babysit a machine. I generally get one to three machines set, and then run them (or have someone else run them and keep rolling along to other machines, which is starting to happen). But I'm not able to do anything when I start the cycles; no setups, inspections, engineering work, et cetera. The machines need attention. And they stop when someone bugs me for something; somebody's tool breaks, somebody needs engineering revisions or additional reference dimensions, someone needs a machine set so they have work.
In your situation, it sounds like having to attend to a machine is somewhat out of the ordinary.
If I could leave and go do more setups or something while a machine bar fed, I could offer a cost difference between the two tolerances; not because .0005" is at all difficult, but because hitting go and walking away shaves off so much of the cost to me per part.
Not that I would offer the difference; the op's post indicates the dude wants to hit 22/part. If someone came in and DEMANDED that price, and I had a hunch it was going to be equivalent to getting paid TWICE my shop rate? Just an example, obviously. I can't make any claims since I have NO idea what the OP is turning or what the cycle times are. I would definitely see if I could work that job into my schedule, if it didn't interrupt whatever else I was doing too much. I get the feeling someone with that attitude is going to be asking for a series of price cuts in the future, and that price buffer would be a good place to bargain from.
My thought process would definitely be a competition between "More jobs running" versus "Fewer jobs, but one (or two) have better margins."
But like I said, I unfortunately don't have the luxury of considering that problem.
Wanna lend me a swiss cnc to fix that? =)
06-26-2009, 07:49 PM #34
06-26-2009, 09:01 PM #35
Ox, my operation is much like Toasty's description.
Other than the EDM, there are very few jobs that run unattended, and even if they are done by " button pushers", I'm still always here to check on the parts or the sounds of the machine.
No matter what, the critical dims are always 100% checked, sometimes with 2 separate instruments. Of course, to date the largest lot I've ever made is under 4000 pieces, but even those had a +/-.0005 OD and ID.
No barfeeders, I or the guys pull the stock after each part, blow chips, clean the cutting area... etc.
Typical work is 80% aerospace, and while the tolerances are absolutely not crazy ( contrary to popular belief ) there is no such thing as a ding, toolmark, scratch ...
The downside is that once you get used to it, it is rather difficult to quote "commerce" parts competitively.
As I've said, a semifinish pass is a norm, so is finish ID, thread, spring ID, spring thread. No chamfer without radius, no cutoff without secondary back. op, no drill-only hole and never to finish with the roughing tool.
All parts are either tumbled, hand deburred or sent out for deburring.
06-26-2009, 09:36 PM #36
Thank you for all of your responses. I have definitely picked up a trick or two and things the be wary of.
The parts were made of A182 F316 and fairly simple. Straight bore at .850 3 inches deep. OD 1" to a 2" shoulder with an undercut in the shoulder. The material was customer supplied, and of course, they only supplied us with just enough to make the job.
My machine is an older Mazak qt-20. It's a good machine but hasn't been treated too well over its life. It can repeat well on +.001 -.0 but I wasn't confident on 5/10ths tolerance.
We primarily use Iscar inserts for our lathe tooling. Rough and finish tools with a free pass programmed for the finish.
As for the price of the parts, I don't get to call those shots.
06-27-2009, 05:41 AM #37
06-27-2009, 09:05 AM #38
Time for the other measurement system?
If your control supports metric, it may be time to use it. If you can offset the machine to the third place in metric, it is equal to .000039" per increment. I would pronounce the figure as 39 millionths
I have always thought that machine controls were biased to metric use. The inch people are missing out on some adjustability if they stay in tenths.
the metric system will allow 12 adjustments inside the tolerance window as opposed to 5 that the inch allows.
I do not know if the machine can resolve a .001 metric adjustment, but if it can, it may help.
Since steel grows at about .000007" per inch of material per degree f°, if the part is at 78°, it will be .000007 X 10 (10 degrees over the 68°f standard to measure at) the increase will be close to one tenth (.00007) so there goes more tolerance.
People that run .00025" tol. just do it, they know the tricks.
The cycle time at $22.00 per part should be able to make money at 4 Parts Per Hour? Sometimes you have to pay for training, invest time to learn, you can't always get the customer to pay for your school.
I love the inch and I will give it up when they pry it from my cold dead hands, but metric is also useful.
I get a kick out of the inch haters, don't hate us just because we can use fractions other than 10ths....
06-27-2009, 09:45 AM #39
Drawings with 0.10", 0.15" etc on them are fine and are a lot easier to work to than 29/64ths for instance.
Ask most 'metric' people who repair things, to make a nice slide fit for something, and they'll say 'a thou clearance'. Not 0.025mm or 25 microns. We can all relate to 'a thou'.
But it does make me smile when companies make a big thing about having gone metric, and their drawings have dimensions all over like 6.35, 12.7, 25.4mm etc.
And material suppliers who ship metric sheet (albeit the standard gauge sizes converted by 25.4....)
06-27-2009, 12:05 PM #40