Tight Tolerance - Machining Aluminum

[Don K]

I am hoping someone can help we with this.

Is it possible to hold +/- .00025 tolerance on a cnc machine? If so, do I drill, ream, or bore these diameters. Based on the education I have had I think we will need some sort of bore gage to inspect these with as well.

 

Please note the depth of 1.31 on 2 of these c'bores.

 

I have inserted a copy of the print. I am quoting this for a future customer.

 

Any advise would be greatly appreciated.

I plan on running these on our Haas VF3 or VM3.

I am merely looking for advice on the correct process to use.

 

[FP1]

Because of that depth I would finish it with a good quality boring bar head (IMO). We had some nice .0002 increment Parlec and Komet heads. If it wasn't that deep I would try to circle mill it.

[Guest]

On a quality machine it will hold that ALL DAY using circle mill. On a HAAS, unless you really baby it, I would suggest using a boring head, reaming it may work as well.

 

JMHO

[Tim Johnson]

Parts like this really show the disavantages of an entry level machine (Hass, Fadal). On a better machine all the features inside the part larger than the Ø.500-Ø.505 can be performed with one tool. I know nothing about Hass, but our Fadal's would have to Bore at least the Ø.99975 and and maybe circle mill the Ø.87545 at around F4. to F10. They would also use at least two end mills for the other features. One possible problem with boring is holding location between the holes (can't see the tolerances). Fadal at least has the feed foward for this. I don't know if the Hass does.

[YoDoug®]

You are really putting too much thought into it, just let FBM decide for you. Heck, you don't want to spend too much time worrying about tolerance while some six year old gets the job done first.

 

 

Kidding aside, our Haas machines can hold .0005 tolerance if you are only checking dia with pins or a single point bore gauge. If you use the CMM though they are usually out of round. If I have a tight bore tolerance I am trying to hold with an endmill I usually try to use a smaller dia. For a 1.0 dia hole If the depth allows I would use a 3/8em and do a helix bore with a small finish step and helix.

[Chris Rizzo]

How many you gotta run? In my experience, you can circle mill it on a haas with cutter comp on and get it within .00025. If you've got to run alot of parts repeatability might require alot of operator attention and offset tweaking. then I'd def say a boring head. For starters I'd recommend a .500 x 1.5 3 flute carbide em for rigidity, circ mill with a few spring passes. (finish pass set to "2" with 0 stepoever).

 

oh, is the vm there finer pitch "more accurate " ballscrew machine? if so run it on that.

 

hth

[GoetzInd]

+1 For boring head

[Guest CNC Apps Guy 1]

I'd bore it on that machine, on a high end machine I'd inerpolate it.

[kunfuzed]

On this subject. How much luck do you guys usually have on your boring heads repeating after a toolchange? I'd be afraid to on this tolerance on our haas machines(even the new one). Usually it's required by the uppers that the operator reset the head each time. (we usually have small runs)

[TR Mfg.]

I would bore these. A good quality boreing head will stay set during a tool change. I might also try reaming, but it may take some trial and error to get the right size reamer.

[1 master]

this is just boring lol

+1 for boring head.

[Jayson Kramer]

I just did a project for harley Davidson 5 months ago that had to hold .0003 and we held .0002 spent almost $3,000 on a boring head and gauges to check it on a Haas VF5.

Worked great.

[Goldorak]

like Jay said , a high end boring head is a must

 

our iscar BH repeat to .0001 at toolchange , make sure that the taper is perfectly clean!

 

when it's very precise (ex: +.0001 -0.0000 ) we rough all the part -.005. then re-run all parts with out toolchange , just bore the hole then change part

 

 

on an okumas hold +-.0002 in circmill is a child play

[Rick Henrickson The Boeing Co.]

Boring head is the way to go, on the toolchange if it is an arm style changer use the large or heavy tool method so it slows the arm down on the toolchange.

[Don K]

I would like to thank everyone for their input. I have been at this programming thing in Mastercam since Version 5 in 1994 or 1995. We have pissing matches going on in our shop currently and you all helped me put those to a halt.

 

Thanks again everyone. You will see me out here again and again because of the help this board has provided.

 

By the way.. I am green to the gills with the lathe package and have never used it in X2 or X3.

Gonna need some help I think.

[Matthew Hajicek - Singularity]

It might be worth talking to the customer about the inspection method. We use customer supplied gauging on some of our most critical stuff, it avoids disputes about whose CMM is more accurate and which inspection method is more correct.

[Rob @ Target Machine]

You are missing the train, my friend. The way to make this decision is based on the machine's backlash. If you can measure .0001-.0002 of backlash - don't bother trying to interpolate the bore. You might get away with it with some customers, but if you want to keep getting their work, do the job right. As a general rule I won't use more than 1/2 of the tolerance given.

[YoDoug®]

quote:

---

You are missing the train, my friend. The way to make this decision is based on the machine's backlash.

---

For each axis in a CNC there are various errors including; yaw, roll, pitch, backlash and a few more that escape me right now. Now compound those errors by the number or axis and spindle conditions and errors and you get to truth of how accurate your machine is. A Renishaw ball bar test will help diagnose most of these.