Spindle Probes Can Automate Trial Machining

An often-overlooked use for spindle probes is in trial machining applications. These applications are useful when a setup person is worried that the cutting tool might not machine a tight-tolerance workpiece attribute correctly on the first try. In this case, an adjustment will be made (commonly using an offset) to ensure that excess material will be left on the attribute.

Columns From: 2/16/2010 Modern Machine Shop

Click Image to Enlarge

The cutting tool will then machine the attribute using the trial machining adjustment. When the cutting tool is finished, the setup person or operator will stop the machine and measure the attribute. They will readjust based on the deviation between the measured attribute’s size and its target. When the cutting tool machines again, the attribute should be at its target dimension.
 
Consider the manual intervention involved in trial machining. In every step, the setup person (or operator, if dull tools are replaced during the production run) must be available to do something. For entry-level people, the procedure is somewhat error prone. Additionally, there are measurements that are difficult or impossible for the operator to take while the workpiece is in the machine.
 
In past columns, I have discussed improving the process of trial machining by programming the trial machining operation. If a setup person or operator can recognize the need for trial machining, surely a programmer should be able to as well. A series of slash codes (block delete function) can be included at the beginning of all trial machining commands. In normal production, the block delete switch will be left on, and trial machining will not be done. However, during setup and after dull tool replacement, the setup person or operator will turn off the block delete switch for trial machining.
 
These techniques facilitate the trial machining process, but they do not automate it. A person must be available to take the measurement. However, a spindle probe will complete the loop, providing a way to automatically measure the workpiece attribute in question.
 
For the setup person or operator to decide whether to trial machine, they must be available to turn off the block delete switch. For fully unattended operation, some kind of logic must be built into the program. This logic should determine when trial machining must be done when running the cutting tool for the first time and when dull tools are replaced.
 
While I don’t provide a complete example, I do provide a bulleted list of the most important considerations for automating this process.
 
In the main program:
O0001 (Main program)
.
.
.
(Critical process that requires trial machining)
N305 T05 M06
N310 G90 G54 S1400 M03
N315 G00 X2.0 Y3.5
N320 G43 H01 Z0.1 M08
/N325 G65 P1000 [list of arguments] (Activates trial machining sequence—note that this method requires a person to flip the block delete switch)
N330 … (Normal machining with tool)
.
.
.
 
The trial machining program (O1000 in our case) must:
 
• Modify the current offset to ensure that excess stock will be left after machining for the first time. This can be done with a G10 command:
 
G91 G10 P5 L11 R0.020 (this command increases offset 5 by 0.020)
 
• Perform the trial machining operation. Machining will probably be identical to what the cutting tool will do to machine the workpiece attribute, but it doesn’t have to be. Often, just enough machining to take a measurement is all that is required.
 
• Measure the machined surface. A tool change will be made to call up the spindle probe. Using the probe manufacturer’s prewritten programs or your own, have the probe measure the workpiece attribute. Most probe manufacturers will place the measured value in a common variable, such as #121.
 
• Calculate the deviation from the target value. The target value can be specified in the main program’s G65 command.
 
• Readjust the offset. Based on the calculated deviation, use G10 to modify the current offset value.
 
• Recall the cutting tool and bring it to its previous position in the main program (line N320 in our example). At the beginning of the measuring program (O1000 in our example), you can use system variables #5001, #5002 and #5003 to store the current absolute position of the machine so that the cutting tool can be brought back to its initial position at this point.
Comments are reviewed by moderators before they appear to ensure they meet Modern Machine Shop’s submission guidelines.
blog comments powered by Disqus
MMS ONLINE
Channel Partners
  • Techspex