Dear Friends,

There is a 5 axis machine with 2 rotary axes (Rotary Table (B) and the one which holds the workpiece with Tailstock (A)) (image attached). Control is Sinumerik 840D pl (powerline) with NCU v6.5 and HMI v6.4. As a result of maintenance and re-assembly, Machine works perfectly with no error but we get to figure out that the final product (Turbine Blade) is not matched with designed one - there is a 0.6 mm difference when measuring depths of cut of both sides of manufactured blade – So, one possibility is that the distance of B axis with respect to the the plane which passes through A axis and tailstock has been changed.

I would like to know how to set the new (modified) origin of intersection of rotary axes or distance between rotary axes A and B and Spindle (the 239.5 and 87.1 numbers in the attached image). Unfortunately, the Sinumerik on this machine doesn’t have any mask or HMI page to set Cycle800, Cycle996, or Traori input parameters (TC_CARR) – due to old version of machine or manufacturer choice, there is no Sinumerik Cycles available but only Manufacturer's Cycles-

Is there a way to set these data in this machines somewhere, such as, in Machine Data in NCU, PLC, or in probably system variables in Cycles?

There was one post regarding this issue for Sinumerik sl, but nothing for Sinumerik pl. any help would be highly appreciated.

Thanks so much for quick response.

Regarding Re-referencing, yes we did. B axis which has absolute encoder has been set via 34210, and A, X, Y, Z axes which have incremental encoders have been set via 34090. The limits were also set.

About realignment procedure, unfortunately machine builder didn’t include anything but some general info such as the one I attached. It only mentions axes limits.

Considering mechanical realignment, our team did their best but still there is some minor differences between new geometry and old one. In our newer machine with newer Sinumerik PL (v7.4), we use page below to set kinematic chain of machine and offset of rotary axes. However, such page is not available on this version of Sinumerik of this machine (v 6.5). Anyway, My question is actually if there is another way to define such offsets in Sinumerik 840D PL v 6.5 like the one we had in Sinumerik PL 7.4 

While only newer controls support the use of TCARR for setting TRAORI parameters, all controls support the original method which uses channel data parameters in the 24500 range.

The current documentation has a cross reference of TCARR to TRAFO5 parameters.  See section 2.7.4 in chapter F2 of the Special Functions manual at  https://support.industry.siemens.com/cs/ww/en/view/109763229

HTH,

SteveA

Dear Steve,

Firstly I should thank you for the help. That was fantastic and give us some idea to go ahead. It took me 1 week to study all this transformation chapter and then I went to machine to see what I can do. Here is the result:

MD24100 $MC_TRAFO_TYPE_1 = 0

MD24500 $MC_TRAFO5_PART_OFFSET_1 [0,1,2] = 0

MD24510 $MC_TRAFO5_ROT_AX_OFFSET_1 [0,1] = 0

MD24550 $MC_ TRAFO5_BASE_TOOL_1 [0,1,2] = 0

MD24560 $MC_TRAFO5_JOINT_OFFSET_1 [0,1,2] = 0

MD20150 $MC_GCODE_RESET_VALUES [24] = 1 (ORIWKS)

MD24570 $MC_TRAFO5_AXIS1_1 [0,1,2] = 0

MD24572 $MC_TRAFO5_AXIS2_1 [0,1,2] = 0

(MD24582 $MC_ TRAFO5_TCARR_NO_1) & (MD24682 $MC_ TRAFO5_TCARR_NO_2) are not even available!!!?

Note: I need to let you know that we have 6 of these machines, all same configuration, only one got under maintenance of rotary axes and only this one doesn’t produce the part same as design. The rest are working with no problem. 

The data above are same for all 6 machines. Results made me more confused. As you can see, all parameters are zero!!?? I am really amazed how other 5 machines work without any problem while there is no transformation information set on these machines? and now I much more wonder how machine kinematics have been defined for this machine by machine builder when actually all kinematic chain data is zero !!??

Not sure if it is related, but your backup archive shows that the control does not have the option set for TRAORI (or tool mangement, for that matter).  Has something happened to cause the loss of option data?

Siemens has a software package (Access MyMachine /P2P) that includes a very useful archive comparison tool called DIFF - see https://mall.industry.siemens.com/mall/en/us/Catalog/Product/6FC58607YC450YA0  It is intended for Solution Line controls but works fairly well for Power Line, except for drive data.

Or, you can copy out parameters from NC Active data and use a text file comparison program to check for differences.

HTH,

SteveA

Dear Steve,

I need to thank you once again for your help.

Yes, as you can see, there is nothing for Traori and it doen't matter that much. All I wanted was sth to define Machine Kinematic inside which surprisingly is not available on this version of Sinumerik PowerLine. 

About your question, I need to say that. No, all machines are same and were like this since first day. As I attached already, Sinumerik version is 6.5 and HMI is 6.4. I checked other Sinumerik versions in our factory and it seems Traori option is available on version above 7.4. So it makes sense why this version doesn't include it but what it doesn't make sense is that how machine builders already define Machine kinematic chains & geometry for these machines with such limited controller? Is that related to ORIWKS set in parameters? meaning that sinumerik doesn't have any idea about machine kinematics and only works based point to point traveling according to part program?

Regarding DIFF, thanks, Yes, I already use it and it is very helpful, both file and folder comparison. But as you said, I can't find Drive MD in that, Seriously where are Drive MDs located in the these ARC files? I even opened with Notpad++ and search for Drive MDs but nothing was there. May I know how you find Drive MD in the arc files of Sinumerik pl?

Well, TRAORI existed long before version 6, so if none of the machines have any of those parameters set, something else is at work.  Could the other machines have a compile cycle that is missing on this machine?  I don't remember exactly where to look, but the Series Startup archive page will have a check box to include compile cycles in the archive if one is present.

Drive data is included on series startup archives only if the check box is selected.  It will make two folders under NC with binary boot files (BOT extension) one for servo drives, one for induction motor drives (VS and HS, maybe?)

When you make an upgrade archive, drive data is always stored in an ascii TEA file format in a folder parallel to NC called DRV.  These can be viewed or extracted with DIFF and are visible using Notepad++

Dear Steve,

I really appreciate your time for explanation. It is really helpful. However, this time I really didn't get what you meant. I even discussed your explanation with two of my colleagues. but none could understand what you meant.The questions are:

1- What do you mean by "compile cycle"?

2- I checked the Series Startup page. Since "compile cycle" is not clear for me, I didn't find anything relevant on this page.

Note 1: I checked all machines cycles. Here is the result:

Standard Cycles: Empty (Strange but yes empty)

User Cycles: It has some cycles but acc. to Machine builder manual, they are measuring cycles. You may see them as attached plus screenshot.

Manufacturer Cycles: Empty

Note 2: This machine comes with a software. The programmer uses that software to design the part and choose machine model in post-processor. Is it possible that Sinumerik here, doesn't do anything at all but an interpolation among coords it gets from generated software code? Still it doesn't solve the problem where machine kinematic chain is defined but I just thought it may help you to have an idea.

About Drive MD, Thanks a million for your very helpful note. Now I found out where such data can be saved. I was actually suspicious about those BOT files but since I couldn't open them, I didn't know what they include but NC Upgrade consists of series of TEA files which exactly they include Drive MDs. Have more questions, but later I will start another post to ask specific question about this matter.

Once again thanks to you for putting precious time on this to read and answer me.

Compile cycles are a way to extend the basic features of the control. You can check for any by:

Diagnosis > Service Display > Version > NCU Version

If there is nothing listed under Loaded Compile Cycles, then you don't have any

In power line controls, Standard Cycles are not loaded by default.  They are supplied in a Cycles folder under Archives in various sets.  If you don't need them there's no point in installing them - they'll just take up program memory space.

Previous generation CNC's did not have any type of kinematic configuration.  For machines with rotary axes, the post processor was used to convert the cutter path into individual axis motions, creating many short blocks taking into account the desired path tolerance.

In this case, the post must know the exact kinematics of the machine.  If this is how your system works, then if all machines use the same part program, all machines must have identical kinematics.  If any are different, then the post must have a machine definition for each distinct machine and create a specific program for each one.