Haas Automatic Tool Presetter — How To

In this video, we'll show you how to use the Automatic Tool Presetter option for Haas CNC turning centers. The Automatic Tool Presetter offers three modes of operation. Manual mode is used for initial setup of tool offsets. Automatic mode is used to update offset values after a tool's inserts have been changed. And Break Detect mode is used to check the cutting face using a preset tolerance for tool wear. To start, press the MDI-DNC button and then program conversational to reach the tabbed menu. Right cursor to the probe tab and press right enter. This brings up the probe menu in manual mode. This turret holds five tools that have no existing offset data. Let's start in manual mode to generate the necessary data for each tool. Check that manual is selected in the op mode box. The turret is at tool position number 12 and therefore the tool number box reads 12. This box will always display the current turret tool position. Enter the offset number you'd like to use for this tool. There are 50 offset numbers available but typically the offset number is set the same as the tool number. Next, set the value for tool tip direction based on the configuration of the tool you're setting. In this case, we are checking a turning insert with its tip in the number 2 direction. We can't enter a value in the tolerance box since we only use that in Break Detect mode. With the turret a safe distance away, move the probe arm into position by pressing F1. With the data entered for tool number 12, you're ready to check the tool position. Handle jog the tool in Z and X until it is approximately a quarter inch diagonally away from the edge of the probe similar to the image displayed in the tool tip direction graphic. If the operator door is open, you will need to hold down cycle start to continue with the touch off cycle or with the door closed, press cycle start. The tool tip will touch off in the Z and X directions and record the offsets. Note that a G-code program is generated in MDI which is used for the tool movement. With the first tool set, move the turret a safe distance from the probe arm and index to the next tool. Continue on to set the remaining offsets. When you are finished setting the offsets for all your tools, don't forget to press F1 to bring the probe arm back to its resting position. With the tools now set, you still need to define your work offset. Start by selecting the desired Z work offset. We're using G54. Using any of the tools you've already probed, touch the tool to the part face and press Z face measure. The distance from the tool probe to the face of the part is loaded in G54 and Z work 0 is now set. Once a tool offset has been set in manual mode, you can update the tool tip position at any time an insert is changed out. Here's how. Access the probe menu and select automatic from the OP mode box. Arrow down to select the tool number you want to check. With the tool number and offset selected, press cycle start. The turret will index to the tool selected in the tool number box and bring the tool to the probe and check the offsets. Repeat this automatic sequence for each tool that needs to be updated. Break detect mode allows you to measure the difference between the initial probe reading for a particular tool insert and subsequent readings after wear or damage may have occurred. The tolerance setting in this mode establishes the allowable wear on a given cutting edge. Select OP mode break detect and the tool number and offset number you used. Now select a tolerance for wear on this particular insert. In this example, we've set this value to 0.004 inches. When the operator presses cycle start, the turret will index to the tool we have entered in the tool number box and the turret will move to the probe and check the insert. If the insert is not within the tolerance set earlier, an alarm will announce that you have a cutting edge that is no longer within specification. When you run break detect mode, a program is generated in MDI. If you paste this into a part program in memory, you will have added that particular break detect routine to your program so that critical tools are measured before they are used. The break detect routine is automatically generated in the upper left side of the MDI screen and is ready to be pasted into a part program. To insert this subroutine into a part program, start by pressing F4. Choose number 1, select create program. Find the program you want to modify. Now simply scroll to the area of the G-code where you want to insert the subroutine and press right enter. Here is a quick demonstration of the break detect routine running within our existing part program. The part program is just ending a drilling operation. Before continuing to a tight tolerance boring operation, the machine will now automatically check that the next tool's insert is within size tolerance. This is particularly useful for checking tools before critical operations. With these three probing modes at your disposal, inputting and checking tool offsets and checking for excessive tool wear, making good parts should get significantly easier.