[roddyf]

What is the cirularity that you guys have found when interpolating a bore with your haas mill?

Thanks

[Geof]

Better than I can measure with a telescopic gauge and micrometer. Certainly less than 0.0005" variation in diameter and probably 0.0002" or even less.

[HuFlungDung]

+/-.0002 or better if the feed is slow.....somewhere between 10 to 20 ipm. The closer the endmill diameter is to the finished hole size, the slower the feed needs to be to keep the effective tangential feedrate within that range.

[roddyf]

Wow, I am getting .013-.014 with a telescoping gauge and a caliper. If I tighten my telescoping gauge in the x and move it to 90 degrees to measure on the Y-axis it rattles in the bore.

[roddyf]

I am running 1/2" 4340 plate waterjet cut .200 smaller than finished diameter. I take 2 cuts with a 1" insert endmill rough cut and a .030 finish cut. Posting out with MCAM.

I just checked a hole that I am drilling with a .413 bit then helix boring with a single flute 1/2 EM to .630 and its better than I can measure.

[Geof]

Wow, I am getting .013-.014 with a telescoping gauge and a caliper. If I tighten my telescoping gauge in the x and move it to 90 degrees to measure on the Y-axis it rattles in the bore.

I do not trust calipers to closer than +/-0.001" but even with that your measurement shows something seriously wrong.

It sounds a bit like something is badly worn or loose in your ballscrew(s), how old is your machine.

[roddyf]

Yeah my machine is 2 months old. I just tried doing a helix bore with the same tool and 4.375" D circle and it came out .001 to .002 out of round.

[Geof]

Two months, this is a warranty issue, get onto your Haas dealer. One possibility on a new machine is that the backlash parameter has been set incorrectly, but whatever it is you need to get it fixed. Check the specs for Haas machines and you will find they have repeatability of 0.0001" and accuracy of 0.0002" so obviously your machine is not up to spec.

[Delw]

Telescopic guages in my opiion are are not a good form of measurement for anything under .002. Most people don't know how to use them correctly. Don't get me wrong you can get .0005 or less out of them repeatally but unless you used them alot dont depend on them. not to mention if there is taper in the bore your going to get false readings

Use a dial bore to check your bores accuratly, if you dont have one Make one out of a flat pcs of alum or steel with a dowel pin or tooling ball and a indicator.

Also chuck a indicator in the spindle and run the z axis to see if you have taper in the bore.


I doubt its the machine but it could be, my first guess is you have taper in the bore, second guess is you need to take 1 or 2 spring pass's with a fresh tool as your tooling is worn out or not cutting correctly.

one other thing to do is since you have cad. start your hole at 30 to 45 degress and run it, this will help eliminate if its the parameters/ballscrews or progam/tooling.
as the ball screws reverse at 0 - 90 - 180 - 270º starting your program at 30 -56 degress will help you find out if its out only on that angles or if its your program or tool pressure

[roddyf]

I did a test with some round stock aluminum, I contoured down to a .750 post and I get readings to .0015" with a mic.

I also don't get any taper on the post but it is aluminum.

I think I will flip my inserts and try interpolating the 3.992 bore again and see what I get.

[Delw]

your getting .0015 with inserts or an endmill on aluminum?

Inserts at least the ones I used, I never used for finishing a bore always followed it up with a solid carbide endmill for finish work.
I know they make them that do finish work now.

You mentioned a big bore Dia. on 1/2" thick stock. just out of curiosity how are you holding this part? how much webthickness do you have around the bore?
I am leaning more towards your set-up and/or tooling is no good or not rigid enough and the parts moving or tweaking.
of coarse its hard to say with out knowing or seeing exactly what you are doing and how.
but I am doubting its the machine from what I've read.

Not trying to say anything bad about your machining skills so dont take that wrong.

Delw

[roddyf]

No offense taken, I am learning. I have a plate that has been waterjetted out with .100 left all around for cleanup.

I have aluminum jaws cut to hold the outside profile, the bore is out to the edge with about 5/8" of material around half of the circle. I am gripping on this thinner material.

I did some program modification and am going to try it again, gonna try a few more passes.

The one problem I thought is the first pass is not pulling the same amount of material all the way around, could be distorting from pressure.

Thanks for the help guys, after profiling that aluminum I feel a lil better about it not being the machine.

[Delw]

thats more than likely the problem.

have you thought about dumping the vices and using a subplate? then clamp the part down with clamps or if there are screw holes. that 5/8 web is awful thin between bore and OD, be very careful with that cause you will get distortion with that big of a bore.


The .0015 on alum isnt good at all that sounds wierd also. I am running location ODs right now that are .600 to the step and 1.250 dia. I mic'd them at .0001 -.0003 with a mic.

Delw

[roddyf]

Anybody know what a haas service guy would do if they came out to look at this problem ie the setup and what kind of part they would want to run and check.

I will do some more tests to see if I am measuring accurately, also will bring my hole mic's to check on monday.

[Delw]

I doubt a service tech is going to tell you about your set-up, you need to find a good machinist in your area and ask them. Haas service techs fix machines not set-ups tooling etc etc.
I know some service techs that would but there company will charge you if the machine is good and its your set-up.

It might be a good idea if you could to post a pic of your setup and let everyone know what tools your using(brand name and type of cutters and post the program so they can read speeds and feeds etc etc.

These guys on this board are pretty smart.

Delw

[dougtyler]

I've run into a problem like this before. My solution was to break the circles, in Mastercam, into 4 parts. This makes Mastercam break the G code into 4 quadrants for a cirlce. Then My holes started coming out round within .0002
My post outputs R's instead of I's & J's. I haven't tried changing the post yet, to see if that would solve the problem. I've just gotten used to breaking the circles.

[Geof]

......I have aluminum jaws cut to hold the outside profile, the bore is out to the edge with about 5/8" of material around half of the circle. I am gripping on this thinner material....

Did you measure before taking it out of the machine? As Delw says it could be a holding problem rather than a machine problem.

Regarding your .75 boss you should get much better than 0.0015" on an OD.

[Delw]

I've run into a problem like this before. My solution was to break the circles, in Mastercam, into 4 parts. This makes Mastercam break the G code into 4 quadrants for a cirlce. Then My holes started coming out round within .0002
My post outputs R's instead of I's & J's. I haven't tried changing the post yet, to see if that would solve the problem. I've just gotten used to breaking the circles.

Wouldnt you be able to tell via the program in the machine if the cut is round or not? or does mastercam make something funky?

[Andre' B]

Wouldnt you be able to tell via the program in the machine if the cut is round or not? or does mastercam make something funky?

By default calculations in mastercam are done to a surprisingly low number of decimal places, in the interest of speed. I believe that can be adjusted someplace.
I have seen on short arcs, less then 0.010 with a large radius, around 3" the center point that MC put in the program was off by something like 0.006 inch. Now if that error puts the center on the wrong side of a quadrant line some controls will do some bad things one I seen would a full circle instead of the short arc. Gets to be hard on tooling.

[samhyto]

The thinner webs on the edges could be lending itself to a distortion issue, depending on your clamping pressure. The bore shouldn't be .013-.014 out. I would put an indicator in the machine and move it to center and check for uniformity of the runout. You could also measure the outside of the part in the vice before and after machining in the event you are getting distortion due to excessive clamping pressure. I would also check the bore and position between rough and finish passes, the part could be moving transversely in the event of insufficient clamping pressure.

We did have an instance on a vf-2SS where the x-axis leadscrew had a locknut issue and it was throwing the x-axis off in rapid but not feed. But I don't think that is the issue here.

Sam