Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Okuma Multus B400 face groove (G72) errors


xarvox
 Share

Recommended Posts

Ive been trying to solve this problem for months now, and i simply cannot get my head around it.

 

I know, its not mastercam related, but i have no where else to go..

 

Im cutting a spiral groove on the face of the chuck, using G72 and alter the start/stop points in mastercam to get the groove wider than the tool.

But the groove isnt uniformly wide from start to bottom.

 

Im using relatively low rpm (120) and only 0,05mm cut depth at a time (5mm wide insert)

 

On other spiral wheels (we make manual chucks), the start (outermost) of the groove is generally tighter the first half turn, then gets wider and keeps same width the rest of the way.

But now i get the opposite error, wider at the start.

 

I belive i checked everything, even painted my insert holder to check if it would scratch against the groove wall, but paint stays unaffected after a full cycle.

 

 

So i ask, beg and pleed with you guys, could anyone please help me solve this?

im clueless and management thinks its an operator issue.. frown.gif

Link to comment
Share on other sites

Hi,

 

Not sure I understand what you are doing here, However

 

G72 is a Compound fixed thread cutting cycle: Transverse

 

So you are using this cycle with a face grooving tool to cut a sprial?

 

Do you have all of this info?

 

G72 X Z K B D U H L E F J M Q

D : First cutting depth

W : Finishing allowance

Q : Number of threads

E : Pitch variation per pitch

J : Number of threads at F value (1 pitch: F/J)

M : M32.....Straight infeed along thread face mode (on left face)

M33.....Zig-zag infeed in thread cutting

M34.....Straight infeed along thread face mode (on right face)

M73.....Thread cutting pattern 1

M74.....Thread cutting pattern 2

M75..... ...Thread cutting pattern 3

Link to comment
Share on other sites

Here´s my program line:

G72 X176. Z24.75 B00 H5.25 D.05 W.05 F10.16 M32 M74

 

The tool is for face grooves, with correct radius for clearance.

 

Im not sure what you mean with "above center height", but my tool insert is below the spindle center if that has anything to do with it..

 

Do you guys want pictures?

Link to comment
Share on other sites

Ah yes pictures always help

 

Sorry but I have a few more questions

 

Can you show us the whole thread cutting code from M321 to the end of that section

 

When you measured the tool where did you measure it to? Top left corner as we look at your pic similar to a boring bar? or bottom left similar to an OD turning tool

 

M602 or M603?

 

Is auto calc turned on?

 

What "P" code do you have in the offset register for this tool?

 

Have you tried your code with A different B angle in place of B00?

 

Also try removing the B00 altogether

 

Does your code look something like this

DRAW

N0001 G140

N0002 G20 HP=4

N0003 G50 S3800

NA001

N0020 G20 HP=4

N0021 MT=00101

N0022 M321

N0023 G97 S152 M41 M04 M08

N0024 G20 HP=4

N0025 TL=001001 M602

N0026 G00 X270 Z5

N0027 X60

N0028 G72 X210 Z-13.05 H13.05 D0.4 W0.02 F15 M22 M73 M32

N0029 M05 M09

N0030 G00 X270

N0031 G20 HP=4

N0032 M01

N0033 M02

Link to comment
Share on other sites

I cut in M602, and use the lower corner when offset setting.

 

The picture displays the tool in M603 merely to display the insert.

 

The P column shows "0" for that specific tools, as for most other tools in my register.

 

Auto calc got me confused, i dont know what youre talking about.. :/

 

I dont use M321 for tool change, instead i use M360, witch was programmed for my by the sales tech on-site.

 

Here you go:

 

N1001 G50 S120

N1002 M90

N1003 G20 HP=1 (HOME POSITION)

N1004 MT=02301

N1005 M360

G0 X9999.

N1006M24

N1007M866

N1008G97 G95 G52 S120 M41 M602 BA=0. M175 TL=023023

N1009 M3

N1010/MT=02301

N1011 G18

N1012 G0 Z60.

N1013 X400.

N1014 Z32.

N1015 X360.

N1016 G72 X176. Z24.75 B00 H5.25 D.05 W.05 F10.16 M32 M74

N1017 G0

N1018 X400.

N1019 Z60.

N1020 M05 M174

N1021 M146

N1022 G0 X9999.

N1023 G20 HP=1

N1024 TL=023000

N1025 M24

N1026 M91

N1027 M02

Link to comment
Share on other sites
  • 1 month later...

A update smile.gif

 

we managed to solve this issue by drasticly increasing RPM and use smaller inserts.

 

The multus dropped aprox 20 rpm for the first full and a half rotation just when the tool got contact with the work piece.

 

and appearantly 5mm insert, 120rpm and 0.05mm cutting depth is too much for this machine.

Now i use 260rpm, 4mm insert and 0.1mm (course) and 0.05 (fine).

 

 

So the problem turned out to be the multus, that it doesnt detect and compensate the dropped rpm fast enough..

 

 

A bit of a bummer on a machine this expencive, bought specificly to handle thease types of jobs..

But at least i found a work-around smile.gif

 

Thank you guys for your help smile.gif

Link to comment
Share on other sites

Greg, i dont know how to answer your questions..

 

i know it has a bit bigger motor and chuck compared to the stock config if thats of any help..

400mm chuch and max 2750 rpm, i cant remember the kW, but i can check it tomorrow.

 

where would i configure the chuck dia?

mastercam or machine?

i usually dont fiddle around in the parameters on any of them, but if you tell me where to check i can find out smile.gif

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...