G68.2 program sample?

[Leon82]

if I recall the mastercam numbers when at a-90 for us were short by 70mm which is how far below the cor the table is. this is if you are analyzing a hole while in position

[huskermcdoogle]

48 minutes ago, sgargaly said:

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

It could, and it couldn't....  It will depend on how you setup your planes in Mastercam and how the post interprets that based on the miscellaneous integers or post settings.

Sorry for the it depends answer.  The "basic" purpose of G68.2 is to put all programming in terms of whatever toolplane you define with the G68.2 line.  AFAIK there are more than just two different schools of thought on how to implement it with a Mastercam post.  This is not taking into the differnt definition methods, I am just talking origin and orientation shift of the toolplane paths.  Whether you use euler angles, roll-pitch-yaw, three points, two vectors, or projection angles, well that's a whole other subject in itself.  Fun math exercises for any implementations of those.  Some are far easier to grasp and visualize than others, some are far easier to implement, but are harder to visualize.

Look and report back on machine parameters 19696 bit 5, 19680, 19681, 19746 bit 4.  This should help us understand what the machine is looking for.

[sgargaly]

Here are the parameters:

para. #19746 = 0 1 0 1 0 0 0 0

          #19696 = 0 1 0 0 1 0 0 0

          #19680 = 12

          #19681 = 4

I hope this helps..

[huskermcdoogle]

I should have had you continue giving more parameters, so far it looks right, basically the coordinates follow the table based on 19696 and 19746.  Now that said, what do you have in 19608 bit 2, I am guessing that is set to 0?  If this is the case, then the position changing is normal.  If you don't want that you can change it, but it will be harder to keep track of where you are so to speak.  Anyway, with the settings so far you should be able to program as if the coordinates are fixed to the rotary table platten.  For purposes of G68.2 this would mean the origin shift (XYZ words on the G68.2 line) would be in those coordinates which would match the machine coordinates when the table is at B0 C0.

[crazy^millman]

8 hours ago, huskermcdoogle said:

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

You can, but don't have to.

[sgargaly]

Do you need G68.2 if you use G54.4?

I have taken screen shots of the  positions at each stage:

First is the start pt of X3.0 and Z15.77254 (machine is at Z home pos.)

Next is at the G68.2  which equals X15.77254 and Z-3.0.

Next is at the G53.1 which equals X21.33974 and Z3.80922.

Last is my G54.1 P20 offset showing X3.31879 Y-7.59905 Z-15.77254 B-.0097 and C315.760.

When I MDI G69 in the control, the X returns to X3.0 ans the Z returns to Z15.77254.

For a B-90 C0 rotation, the G68.2 line shows I270. J90. and K90.

A sample program that I have from the machine dealer shows I-90. instead.

Will this make a difference and can else anyone verify these values?

[huskermcdoogle]

I270 and I-90 should get you the same result in theory

[crazy^millman]

Okay so your machine has the parameter setup to move the machine when the G53.1 in enabled and you need to make sure when you make your programs you are using a point (Clearance distance or ref point) far enough away to allow the machine the room it needs to move from the programmed point to the machine mapped point.

You are setting your P20 values from where? Are they from home or are they from the center of Rotation? They should be set from home is what I have done on many different machines so I look at those values and they puzzle me as you must have one small machine, but yet the machine travels 6 inches in X. My question si where are you setting the values for your Work Coordinate Zero from? Are they from home or are they from center of Rotation?

I is related to the X axis, J is related to the Y axis and K is related to the Z axis just like you see in the normal output on a machine tool of X,Y,Z the I is normally your A axis Rotation and J is B and Z is C. You might ask well it is only a 5 Axis machine why are there 2 Rotations being called out? Space is Space and you are mapping from a known point to another known point and for the machine to map it it will use whatever is needed supplied to it by the post. I90 would Map the values in a positive direction along the X Axis and I-90 would map them negative along the X axis, but that depends on how the coordinate system is defined in the machine or how you look at it. Do you need to look at it form the Spindle to the table prospective or do you need to look at it from the table to the spindle prospective? That is where you need a good post and process established up front and then you program Top/Top/Top if it is a VMC or HMC Style 5 Axis Trunnion Table/Table. It is a Table/Head and not a Table/Table 5 Axis that is where it get tricky depending on how the builder has defined all the axis of the machine.

Still don't have a clue where you are in the world or what kind of machine this is. Any reason why you can't let us know that information?

 

 

[huskermcdoogle]

1 minute ago, C^Millman said:

Still don't have a clue where you are in the world or what kind of machine this is. Any reason why you can't let us know that information?

He didn't tell us where directly, but it is at least a couple year old robodrill, and he is in the northeast, working with cimquest and methods.

I would like to know the rotary table setup.  That would help tremendously, if it is an ISO standard setup, then so be it, but I agree we can't help much without more details.

[sgargaly]

The machine is a small table Fanuc Robodrill vertical mill, with a B axis tilt (about the Y axis) and a C axis rotate (about the Z axis when the B is at 0 deg) trunnion style table. The rotary table is mounted on the left end of the machine table. My G54.1 P20 coordinate system is currently at the center of rotation of the B and C axis from the machine home position (X0 at left, Y0 at back and Z0 at top). The view perspective is from the spindle down to the table is Z minus dir., X+ toward the right and Y+ toward the back. The B tilting axis is limited to +17 degrees  (X- dir.) and -107 degrees (X+ dir.) while the C rotary axis has no limit (+/-360 degree rotations).

I hope this helps.

[crazy^millman]

1 minute ago, sgargaly said:

The machine is a small table Fanuc Robodrill vertical mill, with a B axis tilt (about the Y axis) and a C axis rotate (about the Z axis when the B is at 0 deg) trunnion style table. The rotary table is mounted on the left end of the machine table. My G54.1 P20 coordinate system is currently at the center of rotation of the B and C axis from the machine home position (X0 at left, Y0 at back and Z0 at top). The view perspective is from the spindle down to the table is Z minus dir., X+ toward the right and Y+ toward the back. The B tilting axis is limited to +17 degrees  (X- dir.) and -107 degrees (X+ dir.) while the C rotary axis has no limit (+/-360 degree rotations).

I hope this helps.

Okay have you tried using the home position to set the coordinates? What is happening when you are trying to run this on the machine? What is the behavior? Maybe I missed it, but I want back and so far I have not read where what you did and how you did what you did has not worked. You keep putting up examples of screen shots, but where is the tool exactly when you are trying to do this in relation to the part you are trying to machine. Everything can be explained if we have the details to know what you are seeing. All the information you have given is only about 25% of the answers needed to completely solve this problem. I spent 8 months helping a Customer, Fanuc and an OEM get a machine problem sorted with regards to G68.2. Once we did all was good, but between being able to get answers and get on the machine it took that amount of time. It took me going in and being in front of the machine calling and emailing many different people before the problem was solved.

[sgargaly]

On the response with the screenshots,  the top screenshot is the program position X3.0 Y0  and Z15.77254 when the program is started. This is the X and Y pos. relative to the program coordinate system origin and the center of rotation, since they are the same pt. The program next calls the rotation of B-90. and C0. before the G68.2. The next screenshot is after the G68.2 is read. The position screen values change, but the machine doesn't physically move. The next screen shows after reading the G53.1. The position screen changes again, but the machine doesn't physically move. The last screen shows the G54.1 P20 position on the lower right (G54.1 P19 on the lower middle) and the ABSOLUTE pos. display after the G53.1 is read. I don't know if the coordinate system values can help to figure out the position shifts.

[sgargaly]

Sorry for the long delay.

The machine dealer suggested some methods to check the machine's internal pivot position, but the failing G68.2 

option prevented these from working.

Finally, the machine dealer sent a tech out to see our machine's behavior when trying to use G68.2.

The verdict is........

  the parameter values for the X, Y and Z axis were set at the time of install to INCH values when they should have been set to METRIC values.

So, the rotation pt. used to compensate the G68.2 was really far off location, resulting in the large position display change.

Now we know.

Thanks to all who contributed.

[crazy^millman]

13 minutes ago, sgargaly said:

Sorry for the long delay.

The machine dealer suggested some methods to check the machine's internal pivot position, but the failing G68.2 

option prevented these from working.

Finally, the machine dealer sent a tech out to see our machine's behavior when trying to use G68.2.

The verdict is........

  the parameter values for the X, Y and Z axis were set at the time of install to INCH values when they should have been set to METRIC values.

So, the rotation pt. used to compensate the G68.2 was really far off location, resulting in the large position display change.

Now we know.

Thanks to all who contributed.

Yes helps to set the machine up correctly. Thanks for finally coming back and updating what was going on.