tool presetters

[tunitime]

Just purchased 2 LT15M osp7000 machines with tool presetters. Not sure how to use them and where the offsets are stored. Once the presetter numbers are stored somewhere, how do you offset to the part zero? thanks.

[littlerob]

The primary tool needs be 0 on the presetter, if not you can change the parameters to meet your needs. You should set part 0 with your primary tool, then use your presetter to set the length of the other tools. Tool length is determined by the machine, not the part, but the turning tool (for example) length needs to be 0 for obvious reasons.

Robert

[Algirdas]

I will add a little. Workpiece 0 can be wherever You want. You need to set one tool as it's Z axis offset =0 just for convenience. It's good to use rough OD tool, which works always first and doesn't needs to be accurate.
Tool offsets screen You can reach by pushing the OSP work mode button, next to zero offsets. It's very nice to use calculation function of OSP for tool offsets. For zero offsets too.

[OkumaWiz]

If you push the parameter mode button and then fold the touch setter arm down, the sensor setting screen will automatically appear. These positions are independent or float with your zero set, so once set they will not need to be changed.

To set your sensor positions, first use normal manual method to calculate the tool offset. Once the offset is set, press the parameter mode, fold the arm down, approach the sensor with the tool to within about .15", and then press the sensor keypad arrow key in the direction the tool should approach. The software will automatically make sure you are on the right X or Z value and automatically feed the tool to the sensor and calculate the sensor position taking into account the tool offset.

You may need to touch off a turning tool, a boring bar, and a groove tool in order to initially set all 4 sensor directions.

If you did it correctly, a quick check is to immediately go to Tool Data mode, and use the sensor keypad to touch off and calculate your tool offset again. It should not change more than a tenth or 2.

So in summary, calculating positions (offsets) for sensors and offsets for tools follow the same procedure, it just depends on whether you push parameter or tool data mode. Of course, you need to already have a calculated tool if you are setting a sensor.

Best regards,

[tunitime]

Thanks for the reply's. Once I get the machines in here I will try the procedures. I have 30 similar part numbers and I want to use the same tooling and offsets. My plan is to WRITE to the "Z" zero shift and the "C" zero shift in the different programs. That way the tooling will all be set to the same offsets. Does anyone know the codes to WRITE to the machine zero parameters and not SHIFT the parameters? I would need this for both left and right spindles. LT15M OSP7000lL control.
Thanks for the help.
Dave

[OkumaWiz]

Use VZOFZ or VZOFC to set your zero's in the program.

Be sure that they are done in the correct spindle mode and on the correct turret since the same code works for left, right, A and B depending on which mode you are in.

Another way to do this is to use the TOP file created with the DATA PIP function. You can get even more info into a "setup file". We use this to save tool offsets, zero sets, load monitoring settings etc. with each job.

[tunitime]

Don't know a thing about TOP PIP data files. any info would be great.

[Algirdas]

about TOP PIP data files
You love "PIP"? It's needless here. PIP is just an basic input/ output adjustable program.
any info would be great
It's basic text type file. Parameters are numbered by groups and have one letter definitions. Parameter value is a number.
A lot of parameters are accessible only as a data in parameter file. These don't have access through user interface.

[OkumaWiz]

In edit mode press DATA PIP > OUTPUT> type: MD1:PART.TOP

it will ask you "Output Data is?"

Type: "T,O" and you will get all of your Tool Data Information and Zero Sets in a text file named PART.TOP. It is editable, so if you want to change anything or delete some things to shrink the file you can easily do it in the editor.

If you don't type anything after "Output Data is?" you will get all of your Tool Data Information, Zero Sets, and Parameters. Great for backing up a machine before a software reload.

There is a section in your programming manual that explains more clearly what is being output with Data PIP, so you can get really specific and output only the data you want such as "T1,T2" = Tool offsets and Nose comp registers.

I typically give the TOP file the same name as my part Program (ex: ABC.MIN & ABC.TOP) so as to avoid confusion on what job it is for.

Best regards,