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:

HELP WITH G54.4


motor-vater
 Share

Recommended Posts

So I have questions regarding G54.4 with the use of G68.2. More about how to set up the fixture error than anything else. I have never used this feature in all my years and the one time I need it, its laughing at me. I have read the Mori Book, the Fanuc Book, and talked to the Mori Applications Engineer, Aswell as read every thread related to it on the forum, and sadly I still am struggling

 Things I know

·         Fanuc 31iA5 on Mori NMV5000, needing to cheat my B axis (around Y) to deal with some casting indifferences.

·         Feature is equipped on control (not sure about parameters configured)

·         I get a PS0437 Alarm when I try to add values to the b, c, B, C. But seems to only happen with g68.2,  G43.4 seems to work but does not go to the right area of the part

·         I have a Postability post that has a switch and will output G43.4 Pn

Questions I have

·         Should I post from COR ( I don’t wanna! )

·         But if I do use and use probing to find error form COR, I use those values in fixture error?

·         When trying to cheat my B axis do I put my error in b, or B1

If I post from my probed datum points, do I

·         Leave G54 set to COR and then put the probed difference in to fixture error? X0, Y-6.2048 Z 12.6935

·         Or do I set G54 to the theoretical probed perfect point and use errors as slight adjustments

What I am trying to accomplish

I need to rotate about the Y so that I can bring 2 features into alignment before cutting, because the back cast surface that supports the part in the fixture is not true to the datum targets its either that or shim and indicate every part into the fixture. It’s a TINY adjustment sometimes a .01 adjustment to the B sometimes a half degree. The program is all 3+2 but also uses B axis to cut a feature that lays at 5 deg. , but requires the C to move 270 deg. I feel like the machine should be able to do this according to the Mori guy, its just a mater of getting it programmed right, posted right, and have the correct error values. There will be more info to follow but ultimately I don’t want to overwhelm the first post.

Here is an example of how my post outputs

(HOME POSITION COORDINATES)
(X0.= CENTER OF CASTING DATUM -B- APROX 0.0 FROM COR)
(Y0.= FACE OF CASTING DATUM -A- APPROX -6.2048 FROM COR)
(Z0.= CENTER OF CASTING DATUM -B- APPROX 12.6935 FROM COR)
(-------------TOOL LIST-------------)
(T#*****DIA.*************************DESCRIPTION*************************)
(T150 1/2 3FLT EMC .030RAD 1.0LOC)
G00 G17 G20 G40 G80 G94 G90 G49
G91 G28 Z0. M05
M11
M69
G28 X0. Y0.
G28 B0. C0.
G54
M01

N150
T150 M6
(T150 1/2 3FLT EMC .030RAD 1.0LOC)
G54
G90 G00 B5. C270.
S10000 M03
G68.2 X0. Y0. Z0. I0. J5. K0.
G53.1
M68
M10
G54.4 P1
X.1 Y3.1985
G43 H150 Z6.3007
M8
Z4.8007
G01 Z4.3007 F25.
X-.1 F80.
Y2.9985
ALL OF THE CUTS...........

Z4.8007 F50.
G00 Z6.3007
M05
G49
M9
G69
G54.4 P0
G53 Z0.
G91 G28 Z0.
M11
M69
G28 B0. C0.
M10
M68
G28 X0. Y0.
M30

Link to comment
Share on other sites
4 minutes ago, motor-vater said:

So I have questions regarding G54.4 with the use of G68.2. More about how to set up the fixture error than anything else. I have never used this feature in all my years and the one time I need it, its laughing at me. I have read the Mori Book, the Fanuc Book, and talked to the Mori Applications Engineer, Aswell as read every thread related to it on the forum, and sadly I still am struggling

 Things I know

·         Fanuc 31iA5 on Mori NMV5000, needing to cheat my B axis (around Y) to deal with some casting indifferences.

·         Feature is equipped on control (not sure about parameters configured)

·         I get a PS0437 Alarm when I try to add values to the b, c, B, C. But seems to only happen with g68.2,  G43.4 seems to work but does not go to the right area of the part

·         I have a Postability post that has a switch and will output G43.4 Pn

Questions I have

·         Should I post from COR ( I don’t wanna! ) NO

·         But if I do use and use probing to find error form COR, I use those values in fixture error? YES

·         When trying to cheat my B axis do I put my error in b, or B1 On the G54.4 Page on the control should only have one Axis not 2 so not sure. I would have to test with 20 or 30 degrees to see.

If I post from my probed datum points, do I

·         Leave G54 set to COR and then put the probed difference in to fixture error? X0, Y-6.2048 Z 12.6935

·         Or do I set G54 to the theoretical probed perfect point and use errors as slight adjustments <--- This would be my preferred method. Let the machine do what it is supposed to do.

What I am trying to accomplish

I need to rotate about the Y so that I can bring 2 features into alignment before cutting, because the back cast surface that supports the part in the fixture is not true to the datum targets its either that or shim and indicate every part into the fixture. It’s a TINY adjustment sometimes a .01 adjustment to the B sometimes a half degree. The program is all 3+2 but also uses B axis to cut a feature that lays at 5 deg. , but requires the C to move 270 deg. I feel like the machine should be able to do this according to the Mori guy, its just a mater of getting it programmed right, posted right, and have the correct error values. There will be more info to follow but ultimately I don’t want to overwhelm the first post.

Answers in RED above.

Link to comment
Share on other sites

Thank for the response I have 2 pages, probably doing it wrong no doubt, I have a fixture offset page, and a work setting error page, I have tried entering values into both with no good result from either. Which on should I be using? The Fanuc Book described using a,b,c So I assumed this page was more what I was looking for.

1785797219_FIXTUREERRORPAGE.jpg.5cb727e0df7c544c4dd2983479287339.jpg

FIXTURE OFFSET PAGE.jpg

Link to comment
Share on other sites

Well reading that is explains what the difference are. a is X rotation, b is Y rotation and c is Z rotation. Then the last two are table rotation. In your case what are you trying to rotate? If you are trying to rotate the A or B axis only then a, b or c would not be the correct choice. If you are wanting to shift the XYZ then you would use XYZ. Now where in my mind it get tricky is where is Zero and where are the features you need to shift based off the relationship to that zero point? to me a, b or c will be rotations along that axis from the work offset. If you have a Feature that is 20" from the work offset then .1 shift might be a rotation along the Y axis if b is used, but it will be from the Work Offset position. If you have a Work Offset point that is in a more controlled place to help work our relationship between what you nee to adjust and where you adjust it from it will be doable, but the larger the distance then the more you will have to understand the relationship of the adjustment amount to the actual shift. at 1" the .1 degree may only mean .0002" difference, but at 20" it could be as much as .02" adjustment. Might need to think about localized offsets for key features and use them to help you dial in parts. To me keeping them in relationship to each other might be easier then trying to add a function  you are not familiar with.

Link to comment
Share on other sites
2 minutes ago, crazy^millman said:

Well reading that is explains what the difference are. a is X rotation, b is Y rotation and c is Z rotation. Then the last two are table rotation. In your case what are you trying to rotate? If you are trying to rotate the A or B axis only then a, b or c would not be the correct choice. If you are wanting to shift the XYZ then you would use XYZ. Now where in my mind it get tricky is where is Zero and where are the features you need to shift based off the relationship to that zero point? to me a, b or c will be rotations along that axis from the work offset. If you have a Feature that is 20" from the work offset then .1 shift might be a rotation along the Y axis if b is used, but it will be from the Work Offset position. If you have a Work Offset point that is in a more controlled place to help work our relationship between what you nee to adjust and where you adjust it from it will be doable, but the larger the distance then the more you will have to understand the relationship of the adjustment amount to the actual shift. at 1" the .1 degree may only mean .0002" difference, but at 20" it could be as much as .02" adjustment. Might need to think about localized offsets for key features and use them to help you dial in parts. To me keeping them in relationship to each other might be easier then trying to add a function  you are not familiar with.

I definitely feel you, And I read it the same way, problem is I need the rotation around the Y (b or B) in order to be able to even get the part in the correct orientation/ relationship to the spindle.  Basically if I indicate and shim the part in the fixture on every part, the features are all perfect to each other when cut. The problem is in setting up the casting. We can make good parts with the program, it just takes 45 minutes to set each one up and I am trying to stream line the process, by hopefully using the functionality of the control.

Link to comment
Share on other sites
16 minutes ago, motor-vater said:

I definitely feel you, And I read it the same way, problem is I need the rotation around the Y (b or B) in order to be able to even get the part in the correct orientation/ relationship to the spindle.  Basically if I indicate and shim the part in the fixture on every part, the features are all perfect to each other when cut. The problem is in setting up the casting. We can make good parts with the program, it just takes 45 minutes to set each one up and I am trying to stream line the process, by hopefully using the functionality of the control.

Make a Test Block and use it to help dial in the process. Put features at 10 and 20 degree angles and then use them as reference to help dial in your process.

  • Like 1
Link to comment
Share on other sites

I see a program format issue if you're getting alarms. Activation order should be as follows on a FANUC 30i Series;

N150
T150 M6
(T150 1/2 3FLT EMC .030RAD 1.0LOC)

G05.1P1
G54
G90 G00 B5. C270.

G54.4P1
S10000 M03
G68.2 X0. Y0. Z0. I0. J5. K0.
G53.1
M68
M10
X.1 Y3.1985
G43 H150 Z6.3007
M8
Z4.8007
G01 Z4.3007 F25.
X-.1 F80.
Y2.9985
ALL OF THE CUTS...........

Z4.8007 F50.
G00 Z6.3007
M05

G50P0
G49
M9
G69
G54.4 P0
G53 Z0.
G91 G28 Z0.
M11
M69
G28 B0. C0.
M10
M68
G28 X0. Y0.
M30

 

JM2CFWIW

:coffee:

lower case letters = error (x, y, z, a, b, c)

UPPER CASE LETTERS = Machine Coordinate angles when error was measured. (A/C, A/B, or B/C)

 

  • Like 1
Link to comment
Share on other sites
2 hours ago, cncappsjames said:

I see a program format issue if you're getting alarms. Activation order should be as follows on a FANUC 30i Series;

N150
T150 M6
(T150 1/2 3FLT EMC .030RAD 1.0LOC)

G05.1P1
G54
G90 G00 B5. C270.

G54.4P1
S10000 M03
G68.2 X0. Y0. Z0. I0. J5. K0.
G53.1
M68
M10
X.1 Y3.1985
G43 H150 Z6.3007
M8
Z4.8007
G01 Z4.3007 F25.
X-.1 F80.
Y2.9985
ALL OF THE CUTS...........

Z4.8007 F50.
G00 Z6.3007
M05

G50P0
G49
M9
G69
G54.4 P0
G53 Z0.
G91 G28 Z0.
M11
M69
G28 B0. C0.
M10
M68
G28 X0. Y0.
M30

 

JM2CFWIW

:coffee:

lower case letters = error (x, y, z, a, b, c)

UPPER CASE LETTERS = Machine Coordinate angles when error was measured. (A/C, A/B, or B/C)

 

I definitely appreciate you chiming in on this James. I know from past threads u have experience with G54.4. I will give it a shot. What about a G49 or will the one that output before the tool change do? Once I get working code I am sure Postability will get it to output correctly. Also If you dont mind sharing a little more, I would love to know which screen I should be using, Fixture offset or the Work setting error screen? Thanks for all willing to contribute

fixture offset.jpg

work setting error.jpg

Link to comment
Share on other sites

Hey Pete...

Any references I make to TWP, assume I'm speaking about Euler Angles.

So the reader's digest version of how these functions interact with one another is this;

The work offset is your part origin. For the function to work properly your origin does NOT need to be COR. If anyone tells you any different, send them packing because they don't have a clue what they are talking about and should NOT be listened to. TWP takes that part origin, does all the calculations based on any info on the G68.2 line so that the control knows were the part/path is at all positions, rotations and orientations. It uses the #19700-#19705 parameters (which are the kinematic positions in metric for your machine) on a Tilt/Rotary (trunion) type machine to do the calculations internally. WSEC is applied before TWP because it needs to make any corrections (linear or rotary) before TWP is activated. 

They are deactivated in the opposite order they were activated.

WSEC is for correcting positional linear and/or angular errors in physical and theoretical axes. So on an A/C VMC, you have X, Y, Z, A, and C with B being your theoretical axis. On your MAM72-35V you have X, Y, Z, B, and C with A being your theoretical axis. On an HMC type trunion machine you would have X, Y, Z, A, and B with C being your theoretical axis. THe theoretical axis is essentially an additional G68 Coordinate rotation on top of the other rotations. It's pretty cool to see X motion in your G-Code but the machine is running XY.

Now, any positional or rotational error corrections go into your WSEC offset table NOT in your regular work offset table. You rregular work offsets work best for linear purposes... rotary purposes in a pinch, but I NEVER do any tilt correction there.

Make sense?

Pete, tell Randy is you would have bought the MAM72-63V instead of that Mori your guys' training would be squared away. When you say it to him smile and wink.... because I am. <laughter>

  • Like 1
Link to comment
Share on other sites

Lol! Well I have heard Rumors that our old Mam 72 might be looking shinny new here real soon, but I would hate to try to stuff this part into that thing, it takes up the entire work area of the 5000's

As to the work offsets, I think I may have added a confusing statement. I am talking about 2 different screens I see past my regular work offsets. I have Work Offsets, then Fixture offset screen, then deeper in the Work setting error screen... So Im trying to figure out which of the 2 secondary offset screens I use? The pictures I included were of the fixture offsets screen, then the  Work Set ER, screen. I'll try to make a better picture set or video tomorrow

Link to comment
Share on other sites
9 hours ago, cncappsjames said:

I'm 99.99999% sure you cannot use G54.2 and G68.2 together. 

G54.2 wants to be G68.2 when it grows up. 

There isn't a single [i][b]good[/b][/i] reason to even have G68.2 and G54.2 on the same machine. 

Pretty sure, I agree with you, I think the G54.4 and G54.4 came Standard with the A5 control. Maybe the 68.2 and 43.4 were options the had to pay extra for. IDK I use 68.2 or G43.4 for everything that gets posted for those machines and have never Had a problem, Can move X,Y,Z and C and where I want with no Problems. Its this Dam B axis That does not want to be lied to..

Link to comment
Share on other sites

When I get my computer open in about 40min, I'll see what else I can dig up. I know when you set you errors, if you don't put in the machine angles you took the measurements at, you won't get what you're after. You should have no tilt or rotary values in your work offset.

  • Thanks 1
  • Like 1
Link to comment
Share on other sites

Since you (presumably) have the MAPPS interface I'm not absolutely certain of the keystrokes to navigate to the WSEC offset table on MAPPS.

On a FANUC interface (Standard, Panel i, or iHMI) it is OFS/SET (Offsets/Settings), right arrow soft-key to WORK SET ER. There will be 8 total screens. The first screen is the common screen. Here you only have X, Y, Z, your Tilt Axis and your Rotary Axis (A/C, A/B, or B/C). (See below (This is Matsuura's overlay on on a FANUC 31i-B5 with iHMI Interface - the stuff around the edges is specific to Matsuura, the gray stuff is the normal FANUC stuff)

 

The next 7 screens are your P1 through P7 G54.4 offsets.

The screens are from a Matsuura MX-330.

Lower case letters are your errors. Upper Case letters are where you put your Machine Tilt and Rotary position when the error was recorded.

Some times you need several rotation angles to get the correct data. If that is the case, you need to leave the Tilt and Rotary angles at 0, then you need to figure out what errors go to which axis as if you were at 0, 0, 0, 0, 0. To explain all the possible scenarios this by writing would take a considerable amount of time. It's on my To-Do list to do a YouTube video to explain it... hoping soon.

Hopefully this at least gets you going.

Common.jpg

G54_4P1.jpg

  • Like 1
Link to comment
Share on other sites

Success Update! Seem to be going in the right direction with the format difference, I am now able to get the G54.4 to run with the G68.2, Thank you James. Now I will have to make some test cuts to really figure out how the errors work but So far the Code I posted, a simple square pocket, calls for a rotation of C90, B5 deg and then linear X and Y moves. But as you will see in the video Adding 1 deg of error to the b on the Work Setting Error, moves the axis' to C78.715 and B5.099 and my liner moves are now traveling along both axis' simultaneously. This is a good thing, the machine is now thinking for itself and correcting for the error.  I will have a few last questions after the excitement wears off but wanted to update those that have contributed.

https://youtu.be/iEKy04TZEAI

 

  • Like 2
Link to comment
Share on other sites

Sweet! That's how it's supposed to work.

The easiest way for me to wrap my head around theoretical axis error is to imagine a coordinate rotation on top of a tilt and rotary position. Once your part is flat (using tilt and rotary axis) it can then rotate to program as needed. AND it (WSEC) works with TCP. 

  • Like 2
Link to comment
Share on other sites

Ran some test cuts today, found a few more format errors. When the post outputs a B0, C0 cut it does not use 68.2 So the G54.4 came after the B0. C0, call and did not move the axis'. Was ezily corrected by adding a B0. C0. after the g54.4. I got a list going for when I reach out to the boys at postabilitly, I know they will get it all dialed. But the one Format error that is killing me is the look ahead, no matter what I do I get some kind of alarm with it. It did not like G05.1 p1 at all alarmed out immediately. Usually the old post always used G05 p10000, So I went with that and it works but always alarms out at the end of a toolpath when trying to turn it off.  G05 P0. I tried moving it around and it always alarms no matter where its at. tried canceling the g54.4 first, didn't like it, tried after, no good

tried the way James showed above, nothing

Without G54.4 my post would output like this, and never had problems

G0 Z4.
G49
G69
G05 P0
M9
M5
M81
M69
M11
G0 G17 G40 G80 G90 G98
G91
G28 Z0
G28 X0 Y0
G90
M01

New post wants to do this and it alarms out

Z-7.1333
M05
G49
G05 P0
M9
G69
G54.4 P0
G53 Z0.
G91 G28 Z0.
M11
M69
G28 B0. C0.
M01

 

Ideas? Thanks Everybody for getting me this far

Link to comment
Share on other sites

My end of tool/end of path before new tool plane looks like this;

G00Z....
(CANCEL HIGH SPEED CYCLE HERE)
G00G90G49G53Z0.0
G69
G54.4P0

......

Never have an alarm.

2 hours ago, motor-vater said:
.....

New post wants to do this and it alarms out

Z-7.1333
M05
G49
G05 P0
M9
G69
G54.4 P0
G53 Z0.
G91 G28 Z0.
M11
M69
G28 B0. C0.
M01

 

Ideas? Thanks Everybody for getting me this far

What line is it alarming on?

Link to comment
Share on other sites

was getting a few depending on format. I should have wrote them down, so I'm just going off memory here for now. Originally it was illegal G68 command, on the G69, then I tried moving the G54.4 above the G49/G69 and started getting an illegal WSEC error it became obvious The G54.4 P0 does not want to be before the G49/G69. So moved that back and tried some other stuff but oddly enough removing the G05 P0 gets rid of the illegal G68 alarm, but why the illegal g68 alarm on a G05 P0 has me scratching my head.  Ill post some shorter cycles tomorrow for more detailed info, But I had that spindle shut down for 4 hours today playing around, so I gotta be mindful of our customers. Lol

While I got you on the hook James I have a question about the error values in the Wrk setting errors.  Try to imagine my part be a U shape, in the machine it is an orientation where rotating around the b axis would turn my U into a C. Now when I first load, I am probing the center of the U for my G54. Thats where the part is programmed from. But Then I must rotate my B axis to get the legs of the U even...... Still with me? Today it took -0.101 deg on the B to get there, So I enter that error into the b on my error page. My question is when I come down and reprobe the center of that U it has Moved/Followed and is now .120 shifted in my X. So do I enter that into the x on the error page aswell, or does it just know to follow cause of the b error adjustment.

I ask cause I almost wonder if I should just find and set my rotational error first, then just probe the Center of my U with the B axis at -.101 to the G54 and be done with it? But as I am typing I am thinking probably not a good idea, but How do I find the theoretical perfect position of the part as it was programmed when it has to be skewed to get to that position. Probably why some would Use COR for this I think. Then all you are measuring are errors, Sorry Long winded I am and I hate to take advantage of your kindness, But Lunch on me sometime when we cross paths...

 

Edit: Just dawned on me I can steal the theoretical perfect numbers outta mastercam, Just create a plane at COR and get the values of my Origin point and enter those into my G54. Then that should make my b and x error values valid. Maybe. LOL If that works I would never need to reprobe my G54 and could spend all my energy on the errors...

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...