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 5 Axis problem

Max_vgl

By Max_vgl,
in Industrial Forum

 Share

Recommended Posts

Max_vgl Newbie

Max_vgl

Posted
Posted

Hello,

I have a problem with my Okuma Mu 400 VA.

We bought this machine a few weeks ago and I ran a few tests on it but it wont make a full 5 axis cut.

I read about TCPC (G169) on Okuma and tried it but it throws an error.

I cant find a solution maybe someone can help me out here? 

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
3 hours ago, Max_vgl said:

Hello,

I have a problem with my Okuma Mu 400 VA.

We bought this machine a few weeks ago and I ran a few tests on it but it wont make a full 5 axis cut.

I read about TCPC (G169) on Okuma and tried it but it throws an error.

I cant find a solution maybe someone can help me out here? 

Will have to get a hold of the application team from whom you bought the machine from and have them come in and give you a break down of what the machine can and cannot do. Where did you get your post to post the code from? What toolpath are you using to make 5 Axis motion for the machine? Was a CDS or 5 Axis Artifact run to prove out the machine? I tell all of our customers getting any new machine make them run a CDS for 3 Axis, 4 Axis part for a 4 Axis and 5 axis part on your machine. Test 20 different items since I have seen to many 5 Axis machines setup and not done correctly. Fought with one customer years ago changing a program for 6 weeks never able to dial some blends in. It wasn't until the applications manager realized they had bumped their machine 1st day and never said anything. He rechecked all the machine parameters and they were off. The told him it was setup that way. He then pulled up the alarm history they thought they had erased and showed them overload condition in Z 1 day after the machine was installed. Then they confessed they were trying it out and bumped the machine. That was the customer on that one, but seen other times where parameters were not configured correctly or options that should have been installed were not. Why a customer should always run a test piece as part of the purchase order with the machine. Funny thing is it helps machine builders get a machine paid for quicker since some companies don't know the first thing about 5 axis. They can take months getting their machine up and running and refuse to pay for it until they make a good part. The test piece serves 2 purposes and helps both sides of the process. The customer and the machine builder. 

  • Like 2
Link to comment
Share on other sites
Max_vgl Newbie

Max_vgl

Posted
  • Author
Posted
4 hours ago, crazy^millman said:

Will have to get a hold of the application team from whom you bought the machine from and have them come in and give you a break down of what the machine can and cannot do. Where did you get your post to post the code from? What toolpath are you using to make 5 Axis motion for the machine? Was a CDS or 5 Axis Artifact run to prove out the machine? I tell all of our customers getting any new machine make them run a CDS for 3 Axis, 4 Axis part for a 4 Axis and 5 axis part on your machine. Test 20 different items since I have seen to many 5 Axis machines setup and not done correctly. Fought with one customer years ago changing a program for 6 weeks never able to dial some blends in. It wasn't until the applications manager realized they had bumped their machine 1st day and never said anything. He rechecked all the machine parameters and they were off. The told him it was setup that way. He then pulled up the alarm history they thought they had erased and showed them overload condition in Z 1 day after the machine was installed. Then they confessed they were trying it out and bumped the machine. That was the customer on that one, but seen other times where parameters were not configured correctly or options that should have been installed were not. Why a customer should always run a test piece as part of the purchase order with the machine. Funny thing is it helps machine builders get a machine paid for quicker since some companies don't know the first thing about 5 axis. They can take months getting their machine up and running and refuse to pay for it until they make a good part. The test piece serves 2 purposes and helps both sides of the process. The customer and the machine builder. 

We had a guy here he help us setting up the machine but only for 3 + 2 machining. I asked him about simultaneous but he wasnt sure if the machine can do that.

Im using a post from Fusion 360. I want to rewrite it for the MU and the only problem is simultaneous machining.

I found a manual for a few 5 axis functions maybe there is something that explains my problem.

Thank you for your help :)

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted
1 hour ago, Max_vgl said:

We had a guy here he help us setting up the machine but only for 3 + 2 machining. I asked him about simultaneous but he wasnt sure if the machine can do that.

Im using a post from Fusion 360. I want to rewrite it for the MU and the only problem is simultaneous machining.

I found a manual for a few 5 axis functions maybe there is something that explains my problem.

Thank you for your help :)

You'll definitely want to get in contact with Okuma.

All "full 5-Axis" Controls require proof of the "machine's physical location". There are Export Control regulations which control this.

You will need someone to check the Parameter values on the machine, and must also check to be sure that Tool Center Point Control (TCP) is:

1.) > Enabled

2.) > Properly configured on the Machine Parameter side

Like all 5-Axis Functions > There is a correct order for calling/nesting the 5-Axis Functions, with other functions like "high-speed machine functions". This means that your combination of 'machine functions' must be called in the correct order (output to the NC Code), and then cancelled in the correct order.

With any of the "True 5-Axis Functions", you must calibrate the Center of Rotation Parameters, and also calibrate the Tool Measuring (Tool Length Offsets). Making the machine cut accurately is always a combination of "correctly configured NC Code" and "set of Machine Parameters and purchased Machine Functions", that work together.

I see so many companies that "have 5-Axis machines", but only do positional work. They do this with a "3-Axis Methodology & Approach", and always have to tweak each individual Work Offset, and Tool Offset, to make a complete part that is "in tolerance". Every time they breakdown the job, and set it back up, they struggle with getting a good 1st Article part, and have to scrap a few parts before the job is back up and running smoothly. It doesn't have to be this way.

 

By using the CALL OO88 Function, and TCP, you can just "set a Work Offset with the Probe", and start cutting.

 

Link to comment
Share on other sites
Max_vgl Newbie

Max_vgl

Posted
  • Author
Posted
22 hours ago, Colin Gilchrist said:

You'll definitely want to get in contact with Okuma.

All "full 5-Axis" Controls require proof of the "machine's physical location". There are Export Control regulations which control this.

You will need someone to check the Parameter values on the machine, and must also check to be sure that Tool Center Point Control (TCP) is:

1.) > Enabled

2.) > Properly configured on the Machine Parameter side

Like all 5-Axis Functions > There is a correct order for calling/nesting the 5-Axis Functions, with other functions like "high-speed machine functions". This means that your combination of 'machine functions' must be called in the correct order (output to the NC Code), and then cancelled in the correct order.

With any of the "True 5-Axis Functions", you must calibrate the Center of Rotation Parameters, and also calibrate the Tool Measuring (Tool Length Offsets). Making the machine cut accurately is always a combination of "correctly configured NC Code" and "set of Machine Parameters and purchased Machine Functions", that work together.

I see so many companies that "have 5-Axis machines", but only do positional work. They do this with a "3-Axis Methodology & Approach", and always have to tweak each individual Work Offset, and Tool Offset, to make a complete part that is "in tolerance". Every time they breakdown the job, and set it back up, they struggle with getting a good 1st Article part, and have to scrap a few parts before the job is back up and running smoothly. It doesn't have to be this way.

 

By using the CALL OO88 Function, and TCP, you can just "set a Work Offset with the Probe", and start cutting.

 

Yeah I think Im going to contact someone cause I dont want to mess up the Parameters.

Thank you.

10 hours ago, Greg Williams said:

What error do you get?

The machine is from germany btw.

And the error is in the line with "G169 ..."

20210706_133147.jpg

Link to comment
Share on other sites
gcode Experienced

gcode

Posted
Posted

This is what a G169 command looks like on our Okuma MU-1000 horizontal 5 axis trunnion machine

This is an OSP200 control 2013 vintage

Note that the G169 line defines all 5 axis X Y Z A and B and includes the tool length offset HA 

N2
(SEMIFINISH FLOOR)
(LEAVE .030 STOCK)
(OPERATION NO - 2)
G116 T58 (1.25 X .25R INGERSOLL 2.75 LOC)
M01
G15 H1
/T8
M404
M11
M21
G00 G17 G90 A-86.219 B17.422 S1528 M03
G00 X.046 Y15.2523
G00 G169 HA X-4.4732 Y3. Z-14.409 A-86.219 B17.422
X-4.4732 Y3. Z-14.409 A-86.219 B17.422
X-4.4732 Y2.4274 Z-14.409
X-4.4851 Y1.8288 Z-14.4467
G94 G01 X-4.493 Y1.4296 Z-14.4719 F80.
X-3.3439 Y1.3606 Z-14.1331 A-86.229 B13.311

 

G56 is not used in 5x toolpaths

also note that the A and B axis are prepositioned prior to defining them in the G169 line

 

 

 

 

  • Like 1
Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted 
(POSTABILITY OKUMA GENOS 460V 5AX)
(DRILL BIT)
(MASTERCAM - 2021)
(MCAM FILE - C:\CUSTOMERS\XXXXXXXXXXX\DRILL BIT\DRILL BIT MACHINING.MCAM)
(POST      - MPPOSTABILITY_OKUMA_Genos_460V_5ax.PST)
(PROGRAM   - TOOL 4.MIN)
(DATE      - 2020.09.23)
(TIME      - 2:17 PM)
(T4   - 1/4 BALL ENDMILL     - H4   - D4   - D0.2500" - R0.1250")
(T2   - 1/4 BALL ENDMILL     - H2   - D2   - D0.2500" - R0.1250")
G00 G17 G20 G40 G80 G90
G00 Z=VPPLZ
N1
(FINISH WALL SECTION TOOTH 1A)
(OPERATION NO - 52)
(OPERATION TYPE - SWARF 5AX)
G00 Z=VPPLZ
T4 M06 (1/4 BALL ENDMILL)
G15 H10
M404
CALL OO88 PX=0. PY=0. PZ=0. PA=-96.0845 PC=323.0572 PH=10 PP=51
G00 G17 G90 X.89187 Y3.22605 (TOP MAPPED)
G15 H10
M11
M27
A-96.0845 C323.0572 S5348 M03
G56 HA
M510
G00 G169 X2.11649 Y1.33059 Z-3.49328 A-96.0845 C323.0572 T2
Z-3.49328 A-96.0845 C323.0572
M08
M51
G94 G01 X2.01361 Y1.19377 Z-3.47504 F60.
X2.01296 Y1.19031 Z-3.47414
X2.01018 Y1.17293 Z-3.4721
X2.00848 Y1.15538 Z-3.47388
X2.00839 Y1.1385 Z-3.47926
X2.0103 Y1.12307 Z-3.48775
X2.01452 Y1.10978 Z-3.49869
X2.02086 Y1.09881 Z-3.51117
X2.01958 Y1.10268 Z-3.49839 A-93.3087 C323.7743
X2.01849 Y1.1068 Z-3.48563 A-90.5325 C324.4874
X2.01759 Y1.11118 Z-3.47287 A-87.7561 C325.1999
X2.01686 Y1.11581 Z-3.4601 A-84.9801 C325.915
X2.0163 Y1.1207 Z-3.4473 A-82.2049 C326.6363
X2.01592 Y1.12585 Z-3.43446 A-79.4309 C327.3673
X2.01589 Y1.12586 Z-3.43435 A-79.4323 C327.367
X2.01586 Y1.12587 Z-3.43424 A-79.4336 C327.3667
X2.01584 Y1.12588 Z-3.43413 A-79.435 C327.3664
X2.0158 Y1.12589 Z-3.43398 A-79.4368 C327.3661
X2.01577 Y1.12591 Z-3.43386 A-79.4383 C327.3658

Here it was mapped with CALLOO88 Positioned the A and C axis then G56 HA was called and then G169 was called like Gcode's example. This was posted for a OSP-300M control last year.

Link to comment
Share on other sites
Greg Williams Contributor

Greg Williams

Posted
Posted

So what does that say in English?

I run pretty much the same as Ron in Metric

 

(POST - OKUMA-MU-TCP)
(POST REV - 8.3)
(DATE - 07-07-21)
(TIME - 08:10)
(MCX FILE - 5AX__2021.MCAM)
(NC FILE - 5AX TEST.MIN)
(T6|EMUGE 12250A |H6)
 
VC200=0.2 (TOOL BREAKAGE TOLERANCE)
M404
G0 G17 G40 G80 G90 G94
G0 G16 H0 Z999.
M11
M27
G0 A0. C0.
(EMUGE 12250A |TOOL - 6|DIA. OFF. - 6|LEN. - 6|TOOL DIA. - 12.)
(TOP FACE 1)
N1 T6(EMUGE 12250A TOOL - 6)
M6
G15 H1
G0 G90 A-63.1049 C19.1142 S4000 M3
CALL OO88 PX=0. PY=0. PZ=0. PC=19.114 PA=-63.105 PH=1 PP=51
G0 X3.582 Y28.217
G56 HA Z101.04
G15 H1
M510 (CAS OFF)
G169 HA
G1 X-30.302 Y98.376 Z20.541 A-63.1049 C19.1142 F15000.
M8
M51
M120
Y32.764 Z-.146
X-27.382 Y24.337 Z-4.67
X-24.462 Y15.911 Z-9.194 F800.
X-24.458 Y15.913 Z-9.195 F1000.
X-24.347 Y15.979 Z-9.246

 

 

  • Like 1
Link to comment
Share on other sites
Max_vgl Newbie

Max_vgl

Posted
  • Author
Posted
23 hours ago, gcode said:

This is what a G169 command looks like on our Okuma MU-1000 horizontal 5 axis trunnion machine

This is an OSP200 control 2013 vintage

Note that the G169 line defines all 5 axis X Y Z A and B and includes the tool length offset HA 

N2
(SEMIFINISH FLOOR)
(LEAVE .030 STOCK)
(OPERATION NO - 2)
G116 T58 (1.25 X .25R INGERSOLL 2.75 LOC)
M01
G15 H1
/T8
M404
M11
M21
G00 G17 G90 A-86.219 B17.422 S1528 M03
G00 X.046 Y15.2523
G00 G169 HA X-4.4732 Y3. Z-14.409 A-86.219 B17.422
X-4.4732 Y3. Z-14.409 A-86.219 B17.422
X-4.4732 Y2.4274 Z-14.409
X-4.4851 Y1.8288 Z-14.4467
G94 G01 X-4.493 Y1.4296 Z-14.4719 F80.
X-3.3439 Y1.3606 Z-14.1331 A-86.229 B13.311

 

G56 is not used in 5x toolpaths

also note that the A and B axis are prepositioned prior to defining them in the G169 line

 

 

 

 

I tried it that way but it wont work. Always the same error.

22 hours ago, crazy^millman said: 

(POSTABILITY OKUMA GENOS 460V 5AX)
(DRILL BIT)
(MASTERCAM - 2021)
(MCAM FILE - C:\CUSTOMERS\XXXXXXXXXXX\DRILL BIT\DRILL BIT MACHINING.MCAM)
(POST      - MPPOSTABILITY_OKUMA_Genos_460V_5ax.PST)
(PROGRAM   - TOOL 4.MIN)
(DATE      - 2020.09.23)
(TIME      - 2:17 PM)
(T4   - 1/4 BALL ENDMILL     - H4   - D4   - D0.2500" - R0.1250")
(T2   - 1/4 BALL ENDMILL     - H2   - D2   - D0.2500" - R0.1250")
G00 G17 G20 G40 G80 G90
G00 Z=VPPLZ
N1
(FINISH WALL SECTION TOOTH 1A)
(OPERATION NO - 52)
(OPERATION TYPE - SWARF 5AX)
G00 Z=VPPLZ
T4 M06 (1/4 BALL ENDMILL)
G15 H10
M404
CALL OO88 PX=0. PY=0. PZ=0. PA=-96.0845 PC=323.0572 PH=10 PP=51
G00 G17 G90 X.89187 Y3.22605 (TOP MAPPED)
G15 H10
M11
M27
A-96.0845 C323.0572 S5348 M03
G56 HA
M510
G00 G169 X2.11649 Y1.33059 Z-3.49328 A-96.0845 C323.0572 T2
Z-3.49328 A-96.0845 C323.0572
M08
M51
G94 G01 X2.01361 Y1.19377 Z-3.47504 F60.
X2.01296 Y1.19031 Z-3.47414
X2.01018 Y1.17293 Z-3.4721
X2.00848 Y1.15538 Z-3.47388
X2.00839 Y1.1385 Z-3.47926
X2.0103 Y1.12307 Z-3.48775
X2.01452 Y1.10978 Z-3.49869
X2.02086 Y1.09881 Z-3.51117
X2.01958 Y1.10268 Z-3.49839 A-93.3087 C323.7743
X2.01849 Y1.1068 Z-3.48563 A-90.5325 C324.4874
X2.01759 Y1.11118 Z-3.47287 A-87.7561 C325.1999
X2.01686 Y1.11581 Z-3.4601 A-84.9801 C325.915
X2.0163 Y1.1207 Z-3.4473 A-82.2049 C326.6363
X2.01592 Y1.12585 Z-3.43446 A-79.4309 C327.3673
X2.01589 Y1.12586 Z-3.43435 A-79.4323 C327.367
X2.01586 Y1.12587 Z-3.43424 A-79.4336 C327.3667
X2.01584 Y1.12588 Z-3.43413 A-79.435 C327.3664
X2.0158 Y1.12589 Z-3.43398 A-79.4368 C327.3661
X2.01577 Y1.12591 Z-3.43386 A-79.4383 C327.3658

Here it was mapped with CALLOO88 Positioned the A and C axis then G56 HA was called and then G169 was called like Gcode's example. This was posted for a OSP-300M control last year.

Hmm thank you I am going to try this one. I thought i cant use CALL OO88 and G169 together.

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
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...