Calling all ENGINEERS

I recently set up a line to produce a similar detail.
200 dia bore with a -0/+ 0.03 tolerance - that's about. 001" for you people who haven't yet discovered metric.
It has 2 dowel holes each side with one located to .03 to the bore centre and the other relative to the first dowel with a pitch tolerance of 0.05
This Is in aluminium so the temperature growth is huge.

I made an aluminium master block to replicate the dowel holes and mounted it to the machine bed with one fixed end. I probe it every cycle and then compensate the position and pitch for each part. This removes thermal growth and any axis inaccuracies relating to the machine. You would need to make it from the same material as your workpiece

When measuring, unless you have temperature compensation on your CMM then you should soak the parts in the room for 24 hrs. Or you drag the CMM onto the shop floor and figure out what the pitch should be at the higher temperature.

Don't worry about the shape of the part, the growth is linear so calculate from the drawing dimension.
 
Last edited:
I remember making a little balsa wood magwood car in shop class.

This is about as close as I've gotten to real machine work.

Also, I didn't win the race. :(
 
Togowack said:
The quantity of the order makes it that much money. We just have to get 6 perfect to this drawing and we get full order quantities. Yes I know about thermal expansion which is why I asked if someone knows about software to help account for it, because of the complexity of the part. Not sure if I should put a picture of it here because it is proprietary.

You're right I should go to CNC zone to discuss although I have friends who will offer better advice instead of waiting around for a random person to reply.

Variations of .0001" are of concern because there are two alignment pins that are .002 and .003 respectively, and then a series of bores sitting between them. This is a single axle tube that transfers the weight of the tractor to the wheels, one side being much larger. The positions of the 2 most internal bores (separated by a core) is also .002" total tolerance zone (and all feature are based on these alignment pins)

Total diameter of this part is 19 inches except a square feature that juts out 4 inches. Depth is about the same.

I am all too aware of thermal expansion, which is why we are ordering instrumentation to watch this. The competitors part isn't to spec either, but they said it's closer. Therefore we couldn't argue to loosen tolerances too much.

So I mean, preparing for the trip and have to assume I will supply all the tools to make 6 parts, and they are using a horizontal mill where they machine the bore using an end mill and the alignment pins and then other tools for clearance bolt holes around the perimeter, then the base turns 180 degrees and the bores are machined on the other side. But the CMM reports (local, not Chinese) indicate the two alignment pins are way off, just about everything else jives.

To me the first step is to make sure the CMM reports are accurate and make sense.
Click to expand...

End milling sounds like the problem. Other options?
 
DeadlyRabbit said:
I don't understand how they need to fly someone over there to solve a problem that people on the floor working with the machines should be able to handle. The job is to make parts within tolerance, if someone can't do that they should be fired.
Click to expand...

Nothing is standard in China, one person has this idea, another that, and money is so important to them you can never trust tool wear. They work in a very low pressure environment with machines scraping and screeching and to them its business as usual - their way of putting in the extra effort is putting plants and flowers all over the machine shop.

Chia_Pet said:
just read this.

sounds like the cnc mill isnt holding tolerance, aka slop in the ball screw, AND it could be in both x and y axis.

are the bore on the same axis as the pins?

if so DO NOT interpolate them( using an endmill) BORE them only.

if you have a decent cnc programmer, you can have him program the machine to come to each point from 1 direction.

for example, if you have 5 holes in various positions from left to right, start the first hole to the far left then move to the very next one right, then the next to the right etc.

do the same for the other axis as well.

this keeps the ballscrew tight as it moves in on direction.

if you have to go BACK to a hole, move PAST it, then back to it in the same direction.

this is standard procedure for a quality precision machinist on a manual machine.

the problem with a cnc machine is that typically you are programming the holes or whatever based on what they are.

say 5-10 mm, holes 3-20mm holes, etc

a sloppy machine is most likely the culprit.


PS: you can check the repeatability of the machine by putting in a dial indicator and toughing off the side using the manual controls. zero the dial on the part, move off it whatever distance using the machine coordinates, then move back to the same. if the dial isnt back to zero, thats your problem.
Click to expand...

I went through this entire line of thought today, thanks for the pointer I forgot to check for linear interpolation. That was a big no in school too. However the bores align fine on most parts.

Yes Chia I know engineers all too well.

Lots of good reasoning here, I told the boss line boring might be an option.

But had a conference call today and he basically wrote off the challenge of temperature deviations, and the local boss (even though he doesn't have a clue) said he would allow me that much (what much?) as though I was being held to some unknown standard in his head.

Big boss wants to pour a grey iron fixture and use quick change tooling and for me to overhaul the entire production process instead of just producing 6 good parts, which is good. Foundry and pattern labor are basically free and he wants to really impress.

I think the final critical part here is once the part is machined, to insert a dowel pin and use a dial to center the spindle on that location to double check the distance from the bore.

.005" deviation on a diameter of 19" is more than a temperature problem. I also checked the reports this morning and there was no pattern or consistency to the hole locations, they appear completely random.
 
Togowack said:
I went through this entire line of thought today, thanks for the pointer I forgot to check for linear interpolation. That was a big no in school too. However the bores align fine on most parts.
Click to expand...

It's circular interpolation not linear. And if you are trying to do accurate bores using it you will usually fail.

Do what I said and make a master and measure it in controlled temperature so you know exactly what it is. Bolt it on your fixture (at one end only) and clock it up on the bores. You know the actual pitch b/c you measured it in a controlled environment, now see what your machine thinks it is. Adjust your program by the difference and you will be spot on.

If you need it right every time then clock the master and adjust before the finish cut on each pin/bore. For only a few you can use a standard indicator (get a co-axial one if you want to make it really easy). If you need to make hundreds then set it up with an in spindle renishaw probe.

If it is a fanuc controller you usually have G60 for uni-directional movement. It saves you manually programming past each point and coming back to avoid backlash. it automatically moves an additional amount (set by parameter) and back so you always approach from the same direction (like chia suggested). This shouldn't matter if the machine has glass scales or backlash is properly compensated but it cant hurt anyway.

Also get a coolant temperature controller. Don't try to chill it but maintain it at ambient, this provides the least thermal shock both to your machine and workpieces.

This shit is my bread and butter - I'd come down and help if I was in the country.

gl/hf
 
Looks like this:

x43ltz.png


The CMM room is temp controlled so yes Arak that is the basic procedure, measure the part on the machine to assure position at that temp then in the CMM room after 24 hours sitting in there, measure it and adjust the program for the difference

it may help to check the G-codes but again the bores were not an issue on the reports. This picture shows an old fixture idea I had out of gray iron, on which we would mount hardened pads. Then we would use screws to level it properly on the milling table and dial it in manually for a production run.

One of my friends mentioned putting pins in the bottom so it would install without having to dial. But given the mindset of the machinists over there I think quick change tooling is a big enough step.

v3g95i.png


** this is an old idea that illustrates the concept.
 
The part looks pretty straightforward.

I doubt you are getting any distortion from machining pressure. At that size the temperature will definitely affect it and you should compensate for it.

Drill/ream the holes and bore the centre. If there isn't a big budget for special tooling I would definitely use a basic single point tool for the bearing bore in the centre. Still probably cheap enough to get a custom multi insert tool made to rough out the guts of it and produce the couple of clearance/seal bores.

Your problem may be caused by the alignment of the two bores which I would imagine they use as the datum to measure the pin position to. Clock your B axis and make sure you are getting those aligned. With only a small surface area to measure it wouldn't take much to throw that central axis out. That is most likely where the CMM is going wrong as well, especially if it is swivelling the probe between the two datum bores. Check that the calibration program is calibrating in all the swivelled positions correctly.
 
I hope at least the casting is decent, one of the many jobs we have lost to China over the years was a simple pulley. The company was having lots of problems when they got parts, later they found out the casting was being done out in the woods where they just dug a hole in the ground.
 
They are good at pulleys. I don't think axis B is an issue or the bores would be out.

It would be nice if it was a simple center drill issue. Thinking of pre drilling or step drilling the alignment pins to full size gradually so we can be sure of the position of the holes before they reach full size.

We would do this manually for the first part, send to CMM shop and test in 24 hours, adjust the program accordingly, re check position and CMM at 48 hours and should be good to go.

Limitations in china seem to be porosity and experience for me in the foundry is pretty expensive (hotel stay, food = $200 or so a day) so I will have to learn the foundry art slowly. My boss has wanted plans like this but I haven't been able to deliver

I'm going there first week of september, will actually spend the first week of school in China, so no pressure!!
 
Chia_Pet said:
And for the record, dont call an engineer, they work in theory, call for a machinist, they are the ones that make the parts and understand the issues.

NO engineer will know what I just told you unless they learned it from a machinist.
Click to expand...

I hope this was a troll.
 
it really is crazy that togo can find common ground

do anyone want to talk about winemaking
 
You must log in or register to reply here.
Back
Top