On 2/6/2021 at 2:56 AM, cncappsjames said:

Proper program format for probing;

G5.1Q0

G54(Put tilt and rotary addresses and angles ONLY here)

G68.2X0Y0Z0I...J...K...

G53.1

G43H...

Blah, blah, blah

Probe for X, Y, and Z error. Capturing values and writing them to alternate variables that don't get overwritten. Then probe for A error, B error, and C error. Store those off as well. Then write the errors to the WSEC offset variables. The lower case addresses (x, y, z, a, b, c)  in the offset table are the error amounts. The upper case values are the MACHINE angles of the tilt and rotary  where the measurement was taken.

Turn off the probe.

Continue machining.

If any of that you don't understand, I'd reccommend getting in touch with the company that sold you the machine and have their Application Engineer come and go over the process with you. Training for this via forum isn't the best way to approach it. There are machine parameters involved, there is Custom MACRO B involved, there is order of probing hits involved, etc... all things that are extraordinarily hard to do remotely. I know, I do this for a living.

First and foremost, your machine HAS to be set up and configured properly. If that's not squared away first then this is all just a mental exercise.

JM2CFWIW 

Thank you so much. I will try it and if it does not work I will  contact Fanuc. 

4 hours ago, crazy^millman said:

That was my initial thought as well. Why I suggested breaking up each axis and then using them to come up with the end solution. 5 axis probing and coming up with a G43.4 solution is where a CMM Software that can best fit and gives a Matrix solution is the only way I am aware of to do this. No way I am aware of to build the nominal points and then compare the collected points back in an internal macro in Fanuc to then run iterations tests to see what is the best fit of the collected data back to the desired place to then give the 6 degrees of freedom information needed down to the 5 Matrixes needed for the Machine to then adjust to it. Even then most machines require a movement away and back to apply it. If you have moved it then you should re verify that new position is where you expected it to be. Why probe it to collect data and then not verify it to make sure it is where you expected it to be? 

I have been told to try to place the G54.4 X0Y0Z0I#953J#954K-90 after the G68.2, where #953 and #954 are the angles read by the probe. Does it make sense?  

On 2/3/2021 at 7:44 PM, Greg Williams said:

I think this may work if you use Roll, Pitch Yaw G68.2 P1.

I tried it and it did not work.

On 1/29/2021 at 9:24 PM, Colin Gilchrist said:

G68.2 also does not use "Machine Kinematic Angles" for the IJK Vectors.

The angles involved with G68.2 are Euler Angles, and are typically gives as [Z > X' > Z''] Rotations.

Depending on your parameter settings, the rotations can be applied "to the Axis Vector of the Rotated Coordinate System", or "to the Axis Vectors of the Machine Coordinate System (unrotated)".

To further complicate matters, you can also include a "Q" value on the G68.2 line, which can be used to specify the order of axis rotations. Example: Q123, Q132, Q213, Q231, Q312, or Q321.

The easiest way that I figure out the correct codes, is to just use CAMplete. I know that won't work for many people, due to the costs involved, but man that is such a shame. CAMplete is just about the best Post Processor (and simulator, and Machine Control Layer), that I've ever seen.

How can I know if I am appling the rotations to the Axis Vector of the Rotated Coordinate System  or  to the Axis Vectors of the Machine Coordinate System?

I read about the "Q" but I assumed that this is related to the machine and how its order of movements are internally programmed, if not, how can I know if I should use another "Q" different to Q123?

Sorry I my quesions are really simple but I  just started working with axes rotations and the Renishaw probe.

Thank you 

17 hours ago, Colin Gilchrist said:

I hope it does help. These are really great machines if you have the machine configured properly, and have a good Post Processor to generate the codes you need (and in the correct locations).

If you have the option, I would highly recommend CAMplete for anyone doing 5-Axis machining. This software is a Post Processor, Machine Simulation, and Machine Control Layer, all wrapped into one package. While it is certainly possible to get a Post Processor dialed in to support any 5-Axis machine, there are multiple benefits to using CAMplete that a Post Processor just can't provide you. Foremost in my mind, is the fact that CAMplete has agreements in place with the Machine Tool Builders, to get the actual machine CAD models, including any "options", like laser tool measurement, or any other attachment that interferes with the machine's work envelope. You also get the ability to easily use the advanced 5-Axis Fanuc functions, like Tilted Work Plane (TWP), Tool Center Point Control (TCPC), and Workpiece Setting Error Correction (WSEC).

Beyond "code formatting and output" options, CAMplete also includes "optimization" functions, including volume-based feed correction (Volumetric Leveling), and my favorite "Relative Velocity Leveling". This is so much more powerful than just a 'Post Processor'. It actually analyzes the relative velocity of 'each move', and the amount of linear and rotational displacement of each axis, and CAMplete will adjust the feed value on each move, to compensate for the relative velocity of each axis. The effect is magical; it smooths out the linear and rotary motions, so that your "path" doesn't have the "jerks and hesitations", which are all too common with most 5-Axis Post Processors. It isn't the fault of the Post; it has to do with the actual physical configuration and mechanical characteristics of your machine.

I just went through this very issue with a customer having Parameter issues with a 5-Axis RoboDrill (RoboDrill with Tsudokoma Rotary Table), and once we set the Parameters to our "CAMplete Defaults", and then took his part program in Mastercam, and ran it through CAMplete, the results we perfect 'out-of-the-box', with properly formatted NC Code.

Of course there is a bit of a learning curve with CAMplete, but once you get the hang of it, you'll never want to go back to just using a 'regular Post Processor'. And I'm saying this as a guy who loves editing Posts, and has taught Mastercam Post Processor Editing classes. I still love the MP Language, and the flexibility it gives a good programmer, but the advantages that CAMplete provide me make it my "go-to" solution for 5-Axis programming.

I am using the NX postprocessor although I will check CAMplete in detail. 

I have been told that I should convert the angles given by the probe to Euler angles and then include them into the G68.2 as I was doing. Would it work? How can I convert probe angles  into euler angles?

By the way I forgot to say that the Robodrill also has the Tsudokoma Rotary Table installed.  

Thank you

On 1/30/2021 at 12:57 AM, crazy^millman said:

I would think you would have to solve one axis at a time verses solving 2 axis at a time. Compound angles can be very tricky and depending on how you are capturing the points and then doing the math I would expect to see slight variances trying to do at the same time. I would solve one angle and then check. I would then solve and other angle then check I would then recheck that solution to the final results. By breaking up the collection and checking each one then you take any possible compound error that could happen with a skewed probe hit hitting a compound surface.

Then, ¿should I do something like this?

- Probe the angle around X (#953)
- G68.2X0Y0Z0I#953J0K-90
- Probe the angle around X in order to check if the correction was good.
- Probe the angle around Y (#954)
- G68.2X0Y0Z0I#953J#954K-90

Thanks

18 hours ago, Colin Gilchrist said:

G68.2 (TWP) is not meant to "correct misalignment errors" on your machine.

G68.2 is meant to "translate and/or rotate" a Work Offset Coordinate.

G68.2 gives you the ability to set "1 work-offset", and then "tilt/rotate' the table, and have that Work Offset "recalculated" so that the machine is 'tracking your Zero Point' through space. It eliminates the need for you to 'Calculate new Work Offset XYZ Values', every time to rotate/tilt the table to a new orientation.

To properly correct for 'setup errors' on the machine, you'll need to use WSEC (Work-piece Setting Error Correction), or G54.4.

To use WSEC, and TWP, you must first call up your "Active Work Offset".

Once you've called up "G54" (or G55, or G54.1 P22, Etc.), you then invoke TWP or WSEC (often both), and the corrections (WSEC) or the translation/rotation (TWP) is applied, using your Active Work Offset as the starting location.

With WSEC, there are actually up to 8 different WSEC Offsets (P1-P8), which can be used. This allows you to have multiple parts on the table, and allows you to apply a different correction to each one.

Example:

Part #1

G54

G68.2 > Relative to G54, in this example

G54.4 P1   > Relative to G54, but using the "1st set" of corrections

,

,

G54.4 P0

G69

M30

 

Part #2

G55

G68.2 - TWP > Relative to G55 in this example

G54.4 P2  > Relative to G55, but using the "2nd set" of corrections

,

,

G54.4 P0

G69

M30

 

 

Both WSEC and TWP will then use the "Center of Rotation Parameters" (PRM 197000-19705], to track and correct the positions in space.

In order for WSEC to work (and really, to make sure TCP and TWP are working correctly), you must 'Freshly Calibrate' your C.O.R. Parameters.

Thank you very much. I hope I understood it properly (I am a beginner....) and I can try it on monday. 

Hello RaiderX, 

Thank you for your prompt reply. I had aready checked that webpage but I still cannot figure out what I am doing wrong. 

Hello everyone

I am working with a Fanuc Robodrill equipped with a rotary table (4 and 5 axis) and I have to mill a part taking into account that this milling must be performed along the perpendicular direction of the flat upper surface of the part. In order to do it, The machine is equipped with Renishaw inspecton probe with the objective of capturing the real angle around the X and Y axes. After getting those angles we would like to compensate them with the objective of getting said perpendicularity during the machining. I am using the G68.2 but i am not getting good results. 

I am using the following code "G68.2X0Y0Z0I#953J#954K-90" where #953 is the angle read by the probe around the X axis and  #954 is the angle read by the probe around the Y axis.

Is there anything wrong? Should I compensate those angles by using another code? 

I would really appreciate if someone could give me an idea of what I am doing wrong. 

Thank you very much.