Doosan DNM4500 accuracy

Was hoping someone out there who owns a DNM4500 could give me some input on the accuracy of their machines. I currently have a shop full of Haas VF2ss and Vf3ss machines. I have had a lot of struggles holding .001-.002 true pos on a series of aluminum parts (and some 303/304). According to Doosans listed specs, this should be well within the accuracy of a DNM. Is this your experience? Also was looking at a YCM NXV for the same reason, although its a larger slightly more expensive machine.

Anyone out there run both these brands?

This is for both interpolated and drilled/plunged/reamed bores.

I will try to be unbiased but that will be hard since I work for Doosan. And if I said I was unbiased, you wouldn't believe me anyway, LOL. But, in 40 years in the trade, I had heard good things about them. Then I started using them. I have seen a lot of really tight tolerance parts come through here and we were successful in most. Also seen some unrealistic stuff come through here. All I can say is call Able Machine, they are the dealer in your area. Ask for a demo cut. If they don't have a machine, then we do in our showroom. Very capable machines. Also, if you have any specific questions, call me here in New Jersey. I do mostly milling applications.

Paul Anderson
Applications Engineer
Doosan Machine Tools America
973-618-2457

I appreciate the response! I am definitely looking for an end user opinion on the machines. Doing my homework before making recommendations to the brass here. I've connected with Able, but want to hear from someone who doesn't have vested interest in the brand. As you said! I will take it further with Able when I can.

Our machines are a little older, but we have a DNM 500 and two DNM 400 machines. We regularly hold sub .0005" tolerances across a variety of features with no issues. Profile, true position, and tight bores are all pretty reasonable to maintain. We run exclusively aluminum in ours, so not sure how it would hold up with stainless.

The doosans we have are not as well equipped as our mazaks, but that is probably just how we purchased them.

Thank you. Are you able to interpolate +/-.0005 reliably as well? My current setups I can't run production on interpolated holes with any confidence unless they are >+/-.001. We do 90% aluminum anyhow.

I cant think of any jobs right now where we interpolate a bore. For all of our boring we use boring heads.

We do interpolate bosses very frequently and we can reliably hold .0004". Any more than that and we typically grind the parts.

I picked up a new Dnm 4500 in October last year, and I got all the Fanuc options for smoothing/lookahead/anti jerk. I got it to help keep up with my 3d millwork, and it has been great so far (see photo). Accuracy is about as close as I can measure. You cant get finishes like the attached on a machine that cannot accurately control itself, in my humble experience. The acceleration is pretty quick and I find I am using it on production runs when I don't have 3d work waiting. Feed mills, high speed toolpaths, hard milling- so far it performs great no matter what I throw at it. It just cuts nice. And, maybe not as useful for an Alum shop, but it came with thru spindle air, which I love!

Snyphilis said:

Was hoping someone out there who owns a DNM4500 could give me some input on the accuracy of their machines. I currently have a shop full of Haas VF2ss and Vf3ss machines. I have had a lot of struggles holding .001-.002 true pos on a series of aluminum parts (and some 303/304). According to Doosans listed specs, this should be well within the accuracy of a DNM. Is this your experience? Also was looking at a YCM NXV for the same reason, although its a larger slightly more expensive machine.

Anyone out there run both these brands?

This is for both interpolated and drilled/plunged/reamed bores.

Click to expand...

.
i normally run bigger machines with bigger parts. temperature control will effect sizes and position. as well as spindle tram or lean.
.
1) i often will get different size whether i use coolant or no coolant. coolant normally has a chilling effect even though we use a temperature controlled system that maintains coolant temperature to +/- 1 degree F. if your coolant aint temperature controlled than the changes with temperature can be 200% or more. normal for big part to get smaller on one end if cold coolant only getting on the one end of the part. i often see .0003" changes
.
2) spindle lean. visualize spindle at 45 degree angle as you use a longer tool the center of tool tip is off more in the lean direction. so using different length tools there is a different in position from what it would be if spindle was not leaning or out of tram
.
3) many machines cut like higher and too the left from whats indicated. that is bore a hole. use indicator to center on hole. then take boring head .003 smaller and bore into hole making .0005 bigger dia until you see what side of bore it touches first. many a horizontal mill it bores higher and to the left .0005" from expected location. just saying you will never know this if you never test for this. that is what location you get with spindle turning at high rpm compared to indicating. got to do with oil in the bearings
.
4) machine warmup cycle. bigger machine as you warm it up machine itself changes size. also the bearing rails at extreme ends often slightly rusty and by running warmed as moving all the way to the ends it oils and rubs the rust off rails. hard to describe but effects things when measuring .0002 to .0005"
.
5) servo oscillation. often have to program delays after XY move if machine bouncing back and forth .0002 or more its effecting position. also we program to takeup backlash or always come from same direction. cnc might have .0003 backlash and if you dont take it up you get .0003 errors.
.
6) error higher part off the table. often grid shift calibration changes the higher part off the table. got to do with machine alignment quite normal to also get differences in pallets or tables and when pallet brought into position it might not repeat position to less than .0005
.
quite normal to measure grid shift and get different numbers as the machine warms up. usually it changes .0005 or more than on 2nd and 3rd and 4th tests it changes less and less starts to stabilze
.
warpage. big part just unchucking and reclamping finger tight i often measure .0003 to .0020 changes as part springs out of shape. of coarse warpage can be much more if metal not stress relieved

Have your machine calibrated

I am not running large parts but my thermal expansion in our machines is out of control. We have a spindle probe system installed in the machines and I have to stop midcycle to probe the parts and relocate, otherwise the machine may have moved (.003 at its worst) within the span of a single cycle. If the machine sits for any period of time it adjusts back. It's something I don't think I should have to fix.

Thermal expansion is its own issue. Are you in a temp controlled shop? Warm up cycles before starting for the day? A coolant chiller? Mist collector?

thats why machinist run a warmup cycle so machine calibration more stable before finish ops
.
parts changing shape size with temperature can be big problem too
.
newer cnc have temperature sensors on the slides and ball screws to try to compensate for temperature. some cnc have heaters on machine sections to keep areas at warmup temperature all the time whether machine is running or not
.
but many a time i have seen a mill cut lower as spindle and tool holder warms up and gets longer. can run spindle for 5 minutes before finish cut or run path twice to even out the .0005" warmup error. extra cuts often done for holding tighter tolerances
.
often its more a learning curve on using any machine to hold tolerances. but for example if coolant is 10F different temperature that guaranteed will cause problems and not really a cnc issue as much as shop temperature control

Snyphilis said:

I am not running large parts but my thermal expansion in our machines is out of control. We have a spindle probe system installed in the machines and I have to stop midcycle to probe the parts and relocate, otherwise the machine may have moved (.003 at its worst) within the span of a single cycle. If the machine sits for any period of time it adjusts back. It's something I don't think I should have to fix.

Click to expand...

My largest parts have been about 10" x 12". I have not had any issues with thermal growth, but then I am only hard milling dowel locations over spans slightly smaller than that, and at the same time. I sometimes finish parts overnight with 12 hour programs, but that is the same tool doing surface finish work. I do not have any hands on experience with Haas, but I have seen several in other shops. I have not bought one yet.

spock said:

My largest parts have been about 10" x 12". I have not had any issues with thermal growth, but then I am only hard milling dowel locations over spans slightly smaller than that, and at the same time. I sometimes finish parts overnight with 12 hour programs, but that is the same tool doing surface finish work. I do not have any hands on experience with Haas, but I have seen several in other shops. I have not bought one yet.

Click to expand...

.
i have seen backlash issues cause need for always coming from same direction. many cnc have .0003" or more backlash and tilting action of slides when direction changed. many a program i have added extra moves to takeup backlash
.
servo oscillation can cause problems too

had some wicked trouble passing CMM on some .002" T/P bosses on a 2002 VF-3 this year. I was interpolating the diameter followed by radiusing the top edge of the boss (.125dia BTW). In retrospect, I think the radius kellering operation was throwing a burr or something and giving CMM false readings.
I ended up rounding the top of the pin followed by boring the bosses using unidirectional positioning. In the end not sure if it was an interpolation problem or bad order of operations.
but at the end of the day, it held tolerance pretty well.

.001 T/P over 12" alum part? fagetaboutit.

i have often seen parts held in kurt vise too tight and squeezed and when unchucked the round holes werent round no more and dimensions changed cause it wasnt being compressed
.
chucking force does compress parts. often finish cuts are taken at very low clamping force for this reason. using a torque wrench helps too

mneuro said:

Thermal expansion is its own issue. Are you in a temp controlled shop? Warm up cycles before starting for the day? A coolant chiller? Mist collector?

Click to expand...

I should have been more precise. It's less an expansion issue and more a compensation issue. We were jumping .002+ in 10 mins of running and then jumping .002 again if the machine sat for 10 mins. With a lot of rapiding we even saw a .004 jump. It's definitely fixable but requires down time. So now the grass is looking greener if you know what i mean. Want to try something else.

DMF_TomB said:

i have often seen parts held in kurt vise too tight and squeezed and when unchucked the round holes werent round no more and dimensions changed cause it wasnt being compressed
.
chucking force does compress parts. often finish cuts are taken at very low clamping force for this reason. using a torque wrench helps too

Click to expand...

Oh yeah. Having done a lot of plastics and aluminum, the torque handles are essential. Different people have different feels and some parts turn into nightmares. Especially on the kurt high density vises. The middle jaw leans.

Snyphilis said:

I should have been more precise. It's less an expansion issue and more a compensation issue. We were jumping .002+ in 10 mins of running and then jumping .002 again if the machine sat for 10 mins. With a lot of rapiding we even saw a .004 jump. It's definitely fixable but requires down time. So now the grass is looking greener if you know what i mean. Want to try something else.

Click to expand...

It sounds like there is more at play then just temp fluctuation, given those short times.
Given the investment $$ on a different (new?) machine, perhaps you should spend $1k on laser calibration and ball bar testing of your Haas. Looking at the graphs will certainly tell you if there is something obviously mechanical at play.
Fixed a Fadal 6030 this way, years ago that "wouldn't tap" without breaking taps. $80 resolver on Y axis...

A full grid calibration with lasers will find any problems.
Ordinary vmcs are not hand finished like jig bores or makinos etc and need calibration to get rid of assembly geometric errors.
When I worked for Haas the acceptable head tram was worse than what Id clock a old manual mill into.If it was too far out from factory and levelling wouldnt bring it in the head would be shimmed which obviously brings in a head to column error.