G68.2 program sample?

[sgargaly]

Hello!   This may be an old subject, but I can't find what I have been looking for. I am programming a Fanuc Robodrill 5 axis mill (B-C rotary table added).

I am trying to probe each part before milling to establish the part origin pt. and use G68.2 feature to follow the part origin. The G68.2 option was added to the machine last July

and the Mastercam post was finished a couple of months ago. The machine was tied up until last week, so I couldn't try out the option until last week. The rotations output

from the post seem to match examples I have found on the internet and from the machine dealer. The problem happens when I execute the G68.2 line in the control.

The X and Z positions in the ABSOLUTE pos. page switch for a B-90 C0. rotation . The X becomes Z and Z becomes the X pos. I can't find an example of a G68.2 program

output to determine if this is normal.  My post outputs the X, Y and Z in  non-flipped coordinates as they would be in Mastercam . The post writer says this is normal.

The machine dealer says the coordinate rotation is normal and the post should compensate for the position rotation. Neither person sounds very confident or well based

in using G68.2. If you could give examples and advice on the use of G68.2 feature, it would be helpful as the job must go in the machine soon.

Thanks in advance.

 

[Leon82]

On our matsuura when in twp. With the g68.2 then g53.1 i think.I can't remember off my head it uses xyz like normal. 

 

When it detects a 5 axis path it uses tcp g43.4 (I think) and z is y and depending where the rotary is x and z move as x and y would.

 

Is there an example in the yellow manual?

 

Off the top of my head camplete spits out

 

Ac position 

Xy POS

G68.2 I j k x y z

Xyac

G53.1

G43

 

In a tcp path after the g53.1 

G69

G43.4.

I'm going off memory so I could be wrong. I can copy pasta a code snipit tomorrow

 

[civiceg]

https://www.linkedin.com/pulse/fanuc-g682-5-axis-tilted-work-planes-tim-markoski

[jlw™]

9 hours ago, civiceg said:

https://www.linkedin.com/pulse/fanuc-g682-5-axis-tilted-work-planes-tim-markoski

Tim Markoski, the Legend.

[Leon82]

 

I have the order in my first post wrong

G68.2 xyxijk

G53.1

G43

G69 at the end.

You need to call it out each rotation

 

[Leon82]

Its a pain to upload an file so here is the easiest method for me at the moment

[crazy^millman]

13 hours ago, sgargaly said:

Hello!   This may be an old subject, but I can't find what I have been looking for. I am programming a Fanuc Robodrill 5 axis mill (B-C rotary table added).

I am trying to probe each part before milling to establish the part origin pt. and use G68.2 feature to follow the part origin. The G68.2 option was added to the machine last July

and the Mastercam post was finished a couple of months ago. The machine was tied up until last week, so I couldn't try out the option until last week. The rotations output

from the post seem to match examples I have found on the internet and from the machine dealer. The problem happens when I execute the G68.2 line in the control.

The X and Z positions in the ABSOLUTE pos. page switch for a B-90 C0. rotation . The X becomes Z and Z becomes the X pos. I can't find an example of a G68.2 program

output to determine if this is normal.  My post outputs the X, Y and Z in  non-flipped coordinates as they would be in Mastercam . The post writer says this is normal.

The machine dealer says the coordinate rotation is normal and the post should compensate for the position rotation. Neither person sounds very confident or well based

in using G68.2. If you could give examples and advice on the use of G68.2 feature, it would be helpful as the job must go in the machine soon.

Thanks in advance.

 

You said problems. What are those specific problems? What is the machine and the control? Each machine and each builder does it their own way so those parts of the puzzle are important. What did the machine do and how did it handle each line of code as you single blocked the program? What was the distance to go and how much was it off? Was it rotation issues? Was it position issues? Where there alarms that came up? We have helped many OEMS with this over the years and each one is adamant about the process until you show them how to fix the real problem then the answers will change.

[sgargaly]

Thanks for the responses!

I tried the link that civiceg showed in his response. I don't know if that is a head/head machine as mine are table/table machines.

I am not familiar with the differences program-wise. Also, his coordinate systems are located on each face and not on the center of rotation,

so when I initially posted it, I got no G68.2 output since all coordinate views were in the Z axis at home rotation pos.. When I changed the "Working coordinate system"

tool path views to top view, I then got the G68.2 output. The origin pt. is too close to the views to show a noticable coordinate system rotation from the G68.2.

Leon82 sent a sample program with G54.4 in it. This was an option I used on Mazaks a number of years ago, but these machines don't have the option.

The Y axis output seems large, so is that a result of the post compensating for the G68.2 rotation, or is the part located -10.4 from origin?

My machine is a  vertical machine with a  B + C axis rotary table mounted.

The problem I referred to was the X and Z axis swapping coordinates in single block mode at the G68.2 line. The X was 3.8521 and the Z was 15.7736.

After reading the G68.2 line, the X became 15.7736 and the Z became -3.8521. Is this normal? My post doesn't compensate for this rotation.

 Thanks again, but still confused.......

 

[Leon82]

e the 54.4 is somewhat redundant.you can remove it.

 

Make sure your wcs is correct

 

It sounds like you are not using the g53.1?

[crazy^millman]

Does the machine need a ref or mapped point to allow it to do the math for the G68.2? Yes depending on how the part rotates I would expect to see the axis flip like that. What are your 19700 parameters set to? Can you do full 5 Axis with no problem?

[Leon82]

Youneed to find center of rotation and the table half offset and enter it into those parameters. If they are at 0 you are calculating the rotation in outerspace

[crazy^millman]

10 minutes ago, Leon82 said:

Youneed to find center of rotation and the table half offset and enter it into those parameters. If they are at 0 you are calculating the rotation in outerspace

That should have been done by the Machine Builder once the machine was installed, but I have seen this missed and create issues for a customer.

[jlw™]

Every machine/control I have implemented G68.2 on has had to have at least a few parameters set/changed.  On many controls G68.2 will account for deviation from COR, which is why I always use it.  I program parts daily with it.  Send me a message if you want to talk about it more.

[Leon82]

1 hour ago, C^Millman said:

That should have been done by the Machine Builder once the machine was installed, but I have seen this missed and create issues for a customer.

It sounds like they added the option after the fact. 

So the dealer probably ordered it from fanuc and the installer updated the control.

[sgargaly]

 My origin in Mastercam is the center of rotation of the B/C rotary,  TOP VIEW is WCS and my views are as the part looks in the machine. In a test program, I position the tool at X3. Y0 Z6. B-90 C0 and the ABSOLUTE pos page on the control shows these locations. After reading  the G68.2, the X becomes X6. and the Z becomes Z-3. without the machine physically moving. A G69 command sets the positions back to X3. and Z6.  When I command the G53.1, the rotary axis does not move so I think the IJK post output is correct. Does this mean that the post should compensate the X  and Z axis output to X6. instead of X3. and Z9. instead of Z6.? Or, should the post output the same locations as in Mastercam relative to the origin pt and the machine control internally compensates the position? It sounds like a machine control issue. The control is a Fanuc 31i-A5. I have not yet been in touch with Fanuc for an explanation of the G68.2 option behavior. Currently, we segregate the parts into lots with the same location characteristics. We then run the parts with the program that matches the part location in the fixture. There are several programs in the machine to match the variety of  part lots. The plan is to probe every part in the machine, set the coordinate system to that part and  to use the same program by following the new part origin location using the G68.2 option. I have used G54.4 at other shops, which is an easier option to use but this company has only the G68.2.

Thanks again for the responses.  It has been frustrating dealing with the post company and the machine dealer as they have very little experience with these options.

[Leon82]

The numbers will shift when you command the 68.2 and again when the 53.1 if I recall

Parameter 19700- 19705 in the control

They should match your center of rotation.

 

[Leon82]

On a side note I don't understand why g54.4 wasn't an option fanuc controls all that stuff now. Thefanuc  guy would come with his laptop and reflash to control and you have it

[crazy^millman]

2 hours ago, sgargaly said:

 My origin in Mastercam is the center of rotation of the B/C rotary,  TOP VIEW is WCS and my views are as the part looks in the machine. In a test program, I position the tool at X3. Y0 Z6. B-90 C0 and the ABSOLUTE pos page on the control shows these locations. After reading  the G68.2, the X becomes X6. and the Z becomes Z-3. without the machine physically moving. A G69 command sets the positions back to X3. and Z6.  When I command the G53.1, the rotary axis does not move so I think the IJK post output is correct. Does this mean that the post should compensate the X  and Z axis output to X6. instead of X3. and Z9. instead of Z6.? Or, should the post output the same locations as in Mastercam relative to the origin pt and the machine control internally compensates the position? It sounds like a machine control issue. The control is a Fanuc 31i-A5. I have not yet been in touch with Fanuc for an explanation of the G68.2 option behavior. Currently, we segregate the parts into lots with the same location characteristics. We then run the parts with the program that matches the part location in the fixture. There are several programs in the machine to match the variety of  part lots. The plan is to probe every part in the machine, set the coordinate system to that part and  to use the same program by following the new part origin location using the G68.2 option. I have used G54.4 at other shops, which is an easier option to use but this company has only the G68.2.

Thanks again for the responses.  It has been frustrating dealing with the post company and the machine dealer as they have very little experience with these options.

There are some things not being understood about the process and about machine parameters. Mapping a process using G68.2 is to allow the programmer the ability to work with standard programming process for each view not based on the Center of rotation for the machine. Having your Origin on the center of rotation is defeating the purpose of using G68.2. G68.2 is to allow the programmer to use any position on the machine to program their part from and then let the machine do all the heavy lifting to make the program fed into it work. The only real advantage the this process will gain using G68.2 is the ability to use all the canned cycles in different planes that would not be able to other wise.  When the part is being skewed and moved or the head into different 3+2 or even 3+1 or 4+1 positions they may match the standard Axis layouts or they may not. That is where a good post and a good machine will make the work of the programmer easier. The programmer programs all their planes normally then the post converts it to what the machine needs and done. 

The G53.1 depending on what parameter is set to which way will either move the machine or will not move the machine. I have seen many different Fanuc 31i machines and each of them from the each builder have gone about this process their own way. A programmer can go back to their builder and tell them they will take all responsibility to make sure they don't crash the machine by using an external verification program to run all code through. They will run it on the machine having their hand on the feed hold when proving out programs to have it move while the G53.1 move is being called. That might mean telling them the previous 100's of machine they installed and found the way they are doing it is the safest is not acceptable. I am not really sure it will happen, but nothing stopping anyone from demanding it to be the way they want it to be.

G54.4 is a completely different conversation where the operator or setup person is making adjustments on the control for the part not being where they expected it. G68.2 comes directly from the programmer and is meant to map the coordinate system to a new plane based off of the original programmed plane. It is a programming method and approach where as G54.4 is a process to allow the machine to do work for the process to make changes to setup and parts that happens due to it not being like it was programmed originally. They both have their place, but trying to compare G54.4 to G68.2 is not the same thing. Yes one can do what the other does, but the other can not do what the one does. G68.2 allows a programmer to use all canned cycles at different planes where as G54.4 does not allow for this. It allows the machine to make adjustments to the positions the part really is verses where it should be. G54.4 from a programming standpoint is a nice option to have, but you would not going into programming multi-face parts thinking G54.4 will do it all for you on a Fanuc 5 axis machine. That is where the difference is the G68.2 allows the programmer to control a lot more aspects of their programming process where as with G54.4 has its limits.

I am not say each doesn't have their place and understand the frustration here. 5th Axis CGI have helped many customers over the years with this very problem. Sorry the dealer and post builder are not helping, but my experience is there are 2 sides to every story.  Please update us once this is sorted out and let us know what the resolution to the problem were. Have a great weekend.

[sgargaly]

I will be probing each part in the machine to set the origin relative to the actual part location, so I don't think the origin will be exactly at the machine center of rotation. It is going to change for each part. The question I have is : do I set the coordinate system to the new part origin with the machine using the settings in the parameters for the actual machine pt. of rotation, or do I set the coordinate system to the machine pt. of rotation and put the part origin shift on the G68,2 line using macro variables for the XYZ ? Will the G68.2 function work better with the Mastercam origin on the part rather than the center of rotation? These may be questions for the Fanuc tech. to answer.

Thanks again, and have a great weekend as well.

 

[Leon82]

No, you simply probe the part and set g54.

But the center of rotation parameters need to be set.

If the part is 2 inches off, the control will follow it.

 

We program from the face of the rotary. Not my choice but the guy who triained the boss showed him that way and he wants it that way. But i have put vices way off center and it works as intended.  Also you can raise and lower g54 z when you have a shorter dovetail fixture and it will track that point 

[Leon82]

For a rough check indicate the bore on the rotary and check that number to the 19000 parameters .

 

X should be close

Y can be somewhat off depending on the trunnion

[huskermcdoogle]

Wouldn't you typically use G54.4 and G68.2 together in that order?

[sgargaly]

It seems like a machine control issue.  The control is a Fanuc 31i5. The 19700, 19701 and 19702 parameters are set to the index pt. of the rotary. I don't know what other settings should be.  My program origin is the center of rotation of the rotary table B and C axis and I use the TOP VIEW WCS in Mastercam. My tool path views are the same as the part orientation in the machine. I position the machine to X3. Y0  Z6. B-90 and C0 before the G68.2. After the G68.2 is read, the X becomes X6. and the Z becomes Z-3.0 . The table doesn't rotate when the G53.1 is read, so I think the IJK is correct. A G69 command resets the coordinates back to X3. and Z6. If I command a G0 G90 X3. Z6., the machine moves -3.0 in the X axis and 9.0 in the Z axis which is not the same location on the part. Can I assume that the post is not suppose to compensate for this by shifting the X coordinates by 3.0 and the Z by -9. to position to the correct location on the part? Are the program positions the same as in Mastercam relative to the origin (X3. Z6.)  which means no coordinate "flipping" in the machine? Are the XYZ coordinates of the posted program after the  G68.2 line the same as a program posted without G68.2? Neither Cimquest for the post or Methods Machine for the machine can offer any positive feedback as G68.2 seems like an option that is not often used. I have not contacted Fanuc yet.

Thanks to all for the help.

[Leon82]

You want to position after the 68.2 

 

 

 

[sgargaly]

The post outputs XYZ positions after the G68.2.

I would like to know if a program with G68.2 will have the same XYZ moves as one without G68.2?

The post currently outputs the same tool motions with or without G68.2. The only differences are the G68.2, G53.1 and a G69 cancel outputs .

If this seems correct, then I will look at the machine control settings.

The machine is currently busy running production parts with the original program, so machine control test time is hard to come by.

Getting closer to the solution, I think.

Thanks