I use last version of NX 18.104.22.168 mp 01.
From the version 8.5 I have a strange alarm when I use the ISV simulation.
My cnc machine is a 5 axis table-table machine. I customized my files starting from sim08 that is a similar machine.
When I drill, don't care if with the old drilling processor, or new hole machining operations, ISV give this alarm: ALARM 61212.
If I simulate only the drill operation, sometime the ISV doen't give me any error. When I simulate all the operations, the alarm exits and the simulation stops.
I can continue the simulation obtaining a stop at any drill (at example if I drill 5 holes in a part, the simulation will stop 5 times).
I checked a lot of things and trying to use the sim08 OOTB machine, I don't have this message again, so the problem comes from my customization, but I don't really understand what could I do.
I forgot to say that I use ISV simulating the postprocessed program, not the toolpath.
My cnc machine has a Siemens 840D Operate controller (last generation DMG 5axis machine) and the drilling operation use the customized CYCLE81.
Spost drilling and tapping works regularly (spot drilling is using CYCLE81 too).
It's possible that when the first drilling operation is after a milling operation, something is wrong in the class of the tool? Maybe in the .INI files something don't set the right tool type for the operation?
ALARM 61212 in Siemens 840D manual is: "wrong tool for the operation"
If I try to use a mill tool, instead of a twist drill, the alarm don't exits.
within the cycle81 the variable $P_AD holds the tool-type. I guess, that there is something wrong inside your D-Metacode, were the tool type for this variable will be set. Try to take the default implemementation from the sinumerik.ccf.
Please check additional, if you have the variable for tool type set correctly.
In the OOTB example the post write a to_ini.ini file, which contains this.
Loaction of the file: YOUR_CAM_PART_FILE\cse_files\subprog\to_ini.ini
Tool type is variable $TC_DP1[Tno,Dno]=12
I checked the cycle81 in my post and the one in the OOTB sim08, they are exactly the same but sim08 use Powerline cycle, while my controller is the Solutionline version.
I made a test file with a piece where I program a floor wall operation with a mill tool and a drill operation using different types of drill tools and I am obtaining always the alarm. I tried deep holes cycle (cycle83) and I have the same error message.
In the to_ini.ini file I found $TC_DP1[8,0]=200
How can I set it to 12?
Sorry 12 was only any number.
If you have 200 -> 299 this is correct.
Then check what Thomas F is suggesting.
What do you mean for "try to take the default implementation from the sinumerik.ccf"?
I can't find sinumerik.ccf, I found Siemens840D.CCF and Basic.CCF but they are cifrated files, I can't read them.
I tried to change all my .MCF and .CCF files with the last versions, copying and renaming them from OOTB sim08 and now the drilling operation works! But unfortunately I have new problems never seen before.
And I need to modify my machine assembly kinematic model with the axis datas.
I downloaded Machine Configurator but it's the minimal version. I will take a look to the video that explain how to use Machine Configurator to customize my ISV.
Good afternoon ThomasF,
after a weekend of tests and files editing I have solved all the ISV problems except 1 new problem.
I downloaded and carefully installed new MP02 for 9.5.3.
I checked all the new files, the old files that they should write on, and re-checked and re-editing all my customization folder.
- The drilling problem is totally solved, BUT any tool in any pocket of the carrier MUST have the same tool number of the pocket, AND the SAME compensation number (in the post it will be the number after the letter D) used in the post (my post use ALWAYS D1 or D0 to not have human errors). When I add a tool to the carrier, I find always tool number and compensation number local defined, not inherited. I tryed to edit my machine kinematic files and library_dialogs file but I can't solve this problem, I would like that this numbers are always inherited and change automatically if add a new tool or you move one in an other pocket of the carrier. Now I must open and edit any tool before start ISV.
Does the tool have tool numbers applied in the library?
If there are tool numbers applied in the library make sure to change them to zero (0) to enable inheriting.
You may also edit the Tcl script that imports the tools to not set the tool number, so you don't need to remove the tool number when exporting.
Production: NX10.0.3, VERICUT 8.2, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 11.4
Development: C (ITK), .NET, Tcl/Tk Testing: NX12.0 | AWC 3.4 Preparing: NX12.0
Employees of the customers, together we are strong
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide