MILLING EGG SHAPED BOSS ROUND

[M_CODE1]

We are mill a boss on a part that has a tolerance of 14.2539/142523. The boss is out of round .002 after mill it with the finish pass. This part is running on a new Okuma MA 600 HMC.

What are you suggestions to mill it out of round to make it in tolerance. Inspection gave me about 400 points around the entire bore to help tell where it is out at. I know they are using R for the radius instead of I&J, did't know if that would make a difference? Any sugestions would help. Does anyone know what kind of tolerance a new Okuma should be able to hold on this?

 

Thanks

[Tony35]

use I and J not R and it should help never had good luck with R IMO R means rough only

had a job set with R it was out of round .004 changed to I and J out of round was .0005 on a kitamura HX 500 Fanuc 16i

HTH

[3R!< W3NG3R]

I would think a new Okuma would do better then that.

 

Two things to check IMO.

Is the feed to fast on the machine?

and is the feed to fast on the CMM?

 

My brother uses a ziess CMM and has to limit the scan speed or else it will show the part to be WAY out even if it is not.

 

HTH

 

[ 11-20-2008, 03:18 PM: Message edited by: Eric Wenger @ ExpressMan ]

[M_CODE1]

I think I'm goning to tell that subborn bull in the shop, that were going to try I&J, first then go to making the tool path out of round to make it round.

[gms1]

Im with Tony on this. I've got burned using R in the program especially with a nice .1 overlap to the circle for blending. It made a nice dent into the side of the boss I was cutting.

 

IJK only here!

[Goldorak]

if you got the hi-cut option in the machine control, set it to .0001 or .0002

the machine will automaticaly reduce the feedrate to hold the tolerances if it needs

[Tony35]

also you know where you are out of round is it in the axis change direction area? i know its a new machine but maybe the backlash is out of adjustment?

+1 what eric said feed too fast?

if you still have problems i would have it ball bar tested by okuma of course.

there should be no need to program out of round

just some more thoughts

[mchin-pilot]

If it is sculptured surface or out of round as you said. Use point to point toolpath with high/fair density of points (do not use filter that may out put mixture of arcs and lines - it is changing shape of the object if talk of real fineness)

 

Pick the strategy that may allow you to set the pitch of points ( example multiaxis contantZ has that option, and can keep it 3 axis)(If you are driving your cutter from a wireframe, use surface instead)

 

HiCut/Nurbs control is important to set properly too, the new machine should have it.

[John Summers]

Try the old method. Stick an indicator in the spindle of a Bridgeport and tram the boss.

[ATG]

I agree on the I and J's out with the R's.

[jbreth]

We have a shop full of old and new Okumas. Our older Okumas do not have much for memory as some of you know. So we post out with R's to reduce the size of the program. Not saying its right or wrong. The newer Okumas have tons of memory so the program size is not a factor. However we have much success interpolating bosses and bores. We consistently hold tolerances with in .0002 tir. I would concentrate on your FEED rate. If that does not work look at what kind of tool, 2 flt 4 flt, inserted cutter and what kind of holder. Lots of variables can cause out of round. I found the biggest is to fast of feed. Just my 2 cents.

[X-L Engineering Corp]

I'm glad I read this post were do you change that setting? in the config or in the post.

[jbreth]

"I'm glad I read this post were do you change that setting? in the config or in the post."

 

This is what we use when posting out I,J &K's found in the post "General output settings"

 

spaces : 1 #Number of spaces to add between fields

omitseq : yes #Omit sequence numbers?

seqmax : 9999 #Max. sequence number

arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

breakarcs : 1 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

do_full_arc : 0 #Allow full circle output? 0=no, 1=yes

helix_arc : 1 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

[X-L Engineering Corp]

I have a new MpMaster and those settings are no longer thier.

 

control def

spaces : 1 #Number of spaces to add between fields

 

control def

seqmax : 9999 #Max. sequence number

 

in old post

arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

 

in new post

arctype$:2 #CD_VAR Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.,#5 = R no sign, 6 = R signed neg. over 180

 

control def

breakarcs : 1 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

 

control def

omitseq : yes #Omit sequence numbers?

 

control def

do_full_arc : 0 #Allow full circle output? 0=no, 1=yes

 

control def

helix_arc : 1 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

 

this is now arctype in new post and no IJK

arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

 

 

if someone can help me find were to go I would appreciate it

[P_Scott]

Mike,

 

Definitely follow the IJK suggestion and check the feed. You should easily be able to hold the +-0.0008" you need on that machine as long as the feed is right. The IJK output will be more accurate as well. Both those things should allow you to make the boss round within that tolerance. HTH

 

 

Ted,

 

Typically the arc output is selected in the Control Def now. When Control Def is open, look in list on left for Arc topic. Arc Center type is a box about in the middle of this page. To produce IJK output, change the arc center type to something like "Delta start to center" for XY plane, XZ plane & YZ plane. The last two planes are not necessary if your machine doesn't support XZ & YZ arcs but it can't hurt anything to change them all. Do this first for the current program to test it out, then when it works you can change the Control Def from the Settings menu later to have it that way every time you use it. HTH

[Justin Beebe at Folsom Tool]

I just had to switch a job from outputting R's to IJK's this week and when I did the profile of the part came out much more accurate. This was on an older Makino horizontal mill.