Restarting A Program After Breaking A Tap

It's common to have to rerun tools. If you find a problem during the program verification with the eighth tool, for instance, you'll want to restart the program from the beginning of tool number eight rather than having to rerun the entire program just to get back to that point.

Columns From: 8/1/1999 Modern Machine Shop,

It's common to have to rerun tools. If you find a problem during the program verification with the eighth tool, for instance, you'll want to restart the program from the beginning of tool number eight rather than having to rerun the entire program just to get back to that point.

The ability to rerun tools is directly related to how the program is formatted. All information necessary to get the machine up and running (spindle, coolant, offset instating, and so on) must be included at the beginning of each tool command, even for seemingly redundant commands that would carry over from the previous tool if the program is run from the beginning. Most basic CNC courses teach the strict program formatting methods that will allow tools to be rerun. Included in most successful programming methods is an optional stop (M01) at the end of each tool to allow the setup person or operator to easily stop the program to check and see what the tool has done.

While these basic techniques are quite commonly applied, there are circumstances that present special challenges. Most of these cases will require that you consider a change in program formatting. A little ingenuity and foresight can go a long way toward helping you solve tool rerunning problems.

Consider this case of a broken tap: You have thirty holes to tap, but the tool breaks in the third hole. You replace the tap and need to have the control skip the first three holes and proceeding right to the fourth. But you also need the control to read the G84 command in order to have it know how to tap. Here's the program in its original form:

N155 G54 G90 S500 M03
N160 G00 X2.0 Y2.0
N165 G43 H08 Z0.2 M08
N170 G84 R0.2 Z-0.75 F17.6
N175 X3.0
N180 X4.0 Y3.0
N185 X5.0
N190 X6.0
N195 Y2.0

Now, here is the modified program that will give the needed result:

N155 G54 G90 S500 M03
N160 G00 X2.0 Y2.0
N165 G43 H08 Z0.2 M08
N170 G84 R0.2 Z-0.75 F17.6 L0
N175 X3.0 L0
N180 X4.0 Y 3.0 L0
N185 X5.0 Y3.0
N190 X6.0
N195 Y2.0

The L0 tells the control not to machine a hole in the current command. It happens to be the word for this particular control that specifies how many holes must be tapped. (Most controls have some way to specify this). It lets us have the control read and understand how to tap holes (from line N170), but no holes will be tapped until line N190. We include the Y position in line N185 since it's not the same as it is when the first hole is tapped. If Z is changed, line N185 would also require the current R and Z values.

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