Need 5axis fanuc guru

[Piter69f]

We got new NIIGATA HN-50E - horizontal milling with trunnion and we have a lot of issues. I start with understanding new G codes and functions.

Please correct me if I'm wrong:

G68.2 - TWP tilt work plane. It calculates XYZ and angles from pivot point.

G54.2 - Dynamic offset. It will compensate for fixture error, or fixture being off center or having a sub plate. If I put difference between G54 (center of table) to fixture XYZ zero to F-OFFSET, does the machine do all the magic and calculation? If so should I combine G54.2 with G68.2? if not, that means I need my fixture in the center in order to use G68.2?

G54.4 - WSEC Work Setting Error Compensation. It will compensate for misalignment between 4th and 5th axis??? Also can I combine it with G68.2 and/or G54.2?

G43.4 - TCP Tool  Center Point Control. For simultaneously machining. Can I use this code with G54.2 and/or G54.4?

 

Now the biggest issue we have is misalignment between 4th and 5th axis. I understand nothing is perfect and we should put the "error" somewhere into the control but I'm not sure if the "WORK SET ER" G54.4 is for this or we should do it in machine parameters.

 

Currently when we use g 68.2 and we spin the part 180degree we see error of .0074!! We already talk with Niigata USA, and they want us to add the error to our post which doesn't makes sense to me, or use Dynamic offset which also doesn't make sense. Personally I never heard about any misalignment in 5 axis machines, I know there was some but machine just worked fine.

 

Any help and information in this topic much appreciated. 

[Leon82]

The 19700 to 19705 parameters have to be set correctly for them to work.

The parameter should be labeled so x table position get yourself a mini program to bore two holes 180° apart. Visualize which way you have to shift and move at half of the total indicator reading. Then you can run another part and fine tune it.

[cncappsjames]

G54.4 WSEC is what it's name implies Work Setting Error Correction. Ti calculates it's positions from the #19700-#19705 parameters (kinematic center of rotation plus table offsets)Standard offsets handle things in a generally linear fashioned. G54.4 can compensate not only linearly but spatially as well. It's not "like" any other function.

68.2 TWP It calculates it's positions from the #19700-#19705 parameters as well. It calculates it's angles based on type. Euler type angles are best. Rotation around primary Z(I), rotation around primary X(J), then rotation around new Z(K).

G54.2  RTDFO calculates it's positions from either the common offset or the workoffset PLUS the data in the RTDFO table (distance from COR to part origin).

G68.2 is more powerful than G54.2

G43.4 is TCP. It calculates it's positions from the #19700-#19705 parameters also. It is "usually" reserved for rotary type toolpaths, but it's not limited to them.
You may not use G54.2 in conjunction with G43.4. They would conflict.
You may use G54.4 and G68.2 in conjunction with G43.4

The error you speak of is that mm or inch?

Your kinematic positions MUST be correct of you WILL have size and or location error on parts.

You MUST turn things ON/OFF in specific order or else things will not function correctly.

[Piter69f]

Thank you a lot for clearing things out for me. This is really helpful.

 

The error of .0074 is in inches so it is a lot. We are trying to get someone from NIIGATA to come here and re-check everything and set things right, but I want to make sure I understand how it works so I can test it on the spot. We struggle with this for about a year. 

[cncappsjames]

Depending on the machine configuration, #19702 is the usual culprit. 

188 µm a staggering amount of error 

[Piter69f]

I checked the machine parameters and if understand it correctly #19700 - #19702 (Rotary Table) is my center X,Y,Z.

The #19703 - #19705 (Table 1/2 offset) would be adjustment for the center X,Y,Z. ?

Quote

G54.4 WSEC is what it's name implies Work Setting Error Correction. Ti calculates it's positions from the #19700-#19705 parameters

 

Quote

G43.4 is TCP. It calculates it's positions from the #19700-#19705 parameters also. It is "usually" reserved for rotary type toolpaths, but it's not limited to them.
You may use G54.4 and G68.2 in conjunction with G43.4

Does that means if my fixture is 1.00 inch off, for example, on X axis from center then I put 1.00 in the Work Setting Error Correction, and the machine will calculate everything from center of table ( #19700-#19705) with correction of 1.00 on X? or I should just set my G54 as normal an that's all?

Sorry for all the questions but it's hard to figure this things without proper explanation, and the manuals we got from NIIGATA doesn't even cover all this new G codes.

I think I also found where is the error of .0074in. coming from. It looks like they set Z from table tilted 90degre instead of being at 0. I'll play with it whenever the machine is available

 

Thanks again for your help. 

[cncappsjames]

6 hours ago, Piter69f said:

I checked the machine parameters and if understand it correctly #19700 - #19702 (Rotary Table) is my center X,Y,Z.

The #19703 - #19705 (Table 1/2 offset) would be adjustment for the center X,Y,Z. ?

The #19703-#19705 parameters are for when the top center of the pallet are not perfectly mechanically aligned with the intersections of X, Y, and Z centers of rotation respectively.

So for example on a Matsuura MAM72-100H which is a horizontal 5-Axis we have an X, Y, Z, and an A, and B rotary configuration. A rotates around X, and B rotates around Y. A is the primary tilt axis and B is the secondary rotary axis.
#19700 = COR X
#19701 = COR Y
#19702 = COR Z
#19703 = NOT APPLICABLE to machines with A Axis
#19704 = Distance from COR Y to the top of the pallet.
#19705 = Distance from COR Z to the intersection of the imaginary centerline of the rotating pallet.

These parameters HAVE to be correct. If they are wrong, you will chase part deviation until the cows come home and you may never get it. When I'm troubleshooting these issues I get a Master tool... a REAL one not some end mill stuck in a sidelock endmill adapter. The one I use is a BigKaiser BigPlus Master Tool traceable back to NIST. I use ONLY a BigPlus because I want to eliminate variables. A non dual contact tool is a variable. I don;t like variables. They add to the confusion of solving problems... but I digress. Next I measure the Master tool in the machine's tool measurement system. If it is less than 4µm, then I call it good. If it's more than that I recalibrate until it's between 0 and 4µm. I say 4µm because that's the standard accuracy of most tool measurement systems. Once that's judged to be good then I look at the flatness of the table at home. If it's off at all in the tilt or rotary axis I'll reset the 0 on those axes. If it's off more than spec in the theoretical axis I call service. If things are good so far, then I get out the granite square and test bar and check squareness, perpendicularity, etc... if after all that, things are judged to be within spec, then I start figuring out which axes are off. Like I said previously, Z is the usual culprit... at least for the majority of the error.

187.9µm sure seems like an awful lot of deviation. When the machine was new were the head and the saddle in two separate pieces then assembled onsite? Anything over 100µm throws up a red flag for me and I start checking machine geometry at that point to make sure somebody didn't miss something somewhere.

The values that go into the WSEC Table will be the amount of error that is present between the perfect location, tilt, rotation, and orientation of the part/origin and the actual location(x, y, z), tilt(a), rotation(b), and orientation(c) of the part/origin  in addition to the tilt (A) and rotary (B) angles at which the error(s) were measured.

Using the WSEC table or not will depend entirely on the situation and type of error present. If I only have X, Y, Z, and secondary rotary error, I'll typically just use my G54/Work Offset. If I've got primary tilt axis error or theoretical rotary axis error then I will use my WSEC table.

The values going into #19703-#19705 will depend on the kinematics of the machine. I'll speak only to table/table configuration machines here;
A/B kinematic machines will have values in #19704 and #19705
A/C kinematic machines will have values in #19704 and #19705
B/C kinematic machines will have values in #19703 and #19705

The codes you're asking about are NOT Nigata specific functions/codes. They are FANUC functions/codes. They should be present it your yellow FANUC Manuals.
#19700-#19705 information is in the Parameter Manual (30i/31i-B Series - B-64490EN_03)
G43.4, G54.4, and G68.2 are in the FANUC Common to Machining Center/Lathe Operator Manual(s) (30i/31i-B Series - B-64484EN_03)

HTH

[Piter69f]

Thanks a lot for all the information. This put me in to the right course. I think we are getting closer to fix our problem.

[crazy^millman]

On 12/7/2020 at 2:30 PM, Piter69f said:

Thanks a lot for all the information. This put me in to the right course. I think we are getting closer to fix our problem.

So what did you come up with as the solution to your problem?