The Wireless Intuitive Probing System (WIPS) does many tasks. Some of the tasks are known. For example, WIPS makes these known tasks easier:
- Set tool offsets.
- Set work coordinate offsets.
But WIPS does other tasks that you possibly do not know. This document shows you how to use WIPS to do those tasks.
Use WIPS to Make Special Small Programs for Probe Tasks
Haas mills can use WIPS to make special small programs for probe tasks. These small programs are easy to make and easy to operate. WIPS has easy on-screen instructions. Obey the on-screen instructions to make these small programs.
These small programs are frequently used to set offsets when you prepare the machine for operation. You usually operate these small programs in MDI mode. But you can put these small programs into a part program in memory. These are some of the tasks these small programs can do in a part program:
- Do a check for a broken tool before the next cycle.
- Measure a work offset again, before you cut a high-precision part.
- Measure a dimension of a part area. Change the tool offset. Cut the part area again if the dimension is more than a specified tolerance.
Example: Measure a work offset again, before you cut a high-precision part.
This example uses the OMP40-2 probe.
This example puts a special small program into a part program. The part program has these operations:
- Face operation: Use a 0.5 inch 12.7mm end mill (Tool number 1)
- Contour operation: Use a 0.5 inch 12.7mm end mill (Tool number 1)
Do the steps that follow to make the small program. This small program adjusts the G54 X and Y location for a high-precision part. Make the small program from the WORK OFFSET page.
This example is applicable to a mill that has these two components:
- Mill software version M16.05 or higher
- Press MDI/DNC.
- Press OFFSET one or two times to select the WORK OFFSET page.
- Press the UP or DOWN cursor arrow to select the WORK OFFSET used in the program.
- Use the RIGHT cursor arrow to select the PROBE ACTION column. The Probing page shows.
- The part in this example is rectangular block. Select #4 RECT BLOCK.
- Press the RIGHT cursor arrow to go to the WORK PROBE INPUTS.
- Set the values in the X LENGTH, Y WIDTH, and INCREMENTAL Z inputs. Obey the instructions shown on the control to set these values.
- Press INSERT to copy the small program to the CLIPBOARD .
- Do the steps that follow to put the small program into the part program. Press EDIT to go to the part program. Press the DOWN cursor arrow to put the cursor before tool number 1 .
- Press F1.
- Press the LEFT or RIGHT cursor arrow to select EDIT.
- Press the UP or DOWN cursor arrow to select PASTE FROM CLIPBOARD.
- Press ENTER.
- This puts the copy of the small program into the program in memory .
- To operate this small program, you must add some commands to the program in memory. These commands move the probe to the start location of the probing cycle.
- In the T20 M06 block, you possibly must change the T code to put probe into the spindle.
- You must move the probe to the position above the part (G0 G90 G54 X0. Y0.)
- You must enter the tool length compensation for the probe ( G43 H20 Z.5)
- Here is an example of what the small program could be .
Subsequently, when you operate this program, the program does these tasks:
- Before the program starts the operations, the T20 M06 code puts the probe into the spindle
- The probe moves to the G54 work offset location.
- The probe measures the part. Then the program adjusts the G54 X and Y work offsets.
- Then the program machines at this new probed location.
Help to decrease errors on high-precision parts.
This type of small program measures the location of each part that you put into the machine. This corrects for differences that can occur when you put the part in the machine. This helps to decrease errors on high-precision parts.