Siemens Turning Drilling with G95 instead of G94

[Anonymous]

Can any one please suggest how do I modify the post processor of Siemens turning so that the feeds in the program are in feed/rev instead of feed/min? My CNC turning Center does not take G94 and I crashed a drill using G94 . Can i change something in post processor so that the drilling program contains G95 and Feed as feed/rev of the drill parameters? 

[KrupalVala]

Hi @Anonymous ,

Change the unit as an Inches and You will get G95 output. But if you want G95 only in a particular strategy then we need to change a few codes inside the post.

Thanks,

[Anonymous]

Well we use metric system here. I can change the codes in the post
processor if u tell me what needs to be changed.

[Anonymous]

I tried changing the units to inches. But for drilling it still has the feed with G94 as shown as attached.

[KrupalVala]

Hi @Anonymous ,

 I will check and give an update.

Thanks,

[KrupalVala]

Hi @Anonymous ,

To get a G95 code only in drilling, Open your post in any editor. Search below codes and set it from

gFeedModeModal.reset();
  if (currentSection.feedMode == FEED_PER_REVOLUTION) {
    writeBlock(getCode("FEED_MODE_UNIT_REV"));
  } else {
    writeBlock(getCode("FEED_MODE_UNIT_MIN"));
  }

to

gFeedModeModal.reset();
  if (currentSection.feedMode == 0 && getParameter("operation-strategy") == "drill") {
    writeBlock(getCode("FEED_MODE_UNIT_REV"));
  } else {
    writeBlock(getCode("FEED_MODE_UNIT_MIN"));
  }

Now save the post and test it carefully.

Thanks,

[Anonymous]

Thanks for your effort. Really appreciate it. The program now gets the G95
instead of G94 but the feed parameters are the same as with G94. Picture
of the program with the edited post processor attached for your reference.

[image: Screenshot 2020-08-17 at 10.58.16 PM.png]

[Anonymous]

 The program with suggested edits.

[KrupalVala]

Hi @Anonymous,

Sorry for that, Search function onCycle() { in your post and update the codes as shown below,

function onCycle() {
  
  expandCurrentCycle = false;

  if ((cycleType != "tapping") &&
      (cycleType != "right-tapping") &&
      (cycleType != "left-tapping") &&
      (cycleType != "turning-canned-rough")) {
        if ((cycleType == "drilling")){
//Replace above dondition with below, to get feed/rev in holemaking cycles 
//if (getParameter("operation-strategy") == "drill"){ 

    writeBlock(feedOutput.format(getParameter("operation:tool_feedPerRevolution")));
        }else{
          writeBlock(feedOutput.format(cycle.feedrate));
        }
      }

If you are doing drilling (Drilling - Rapid out) operation then only you will get Feed/Rev. Based on your requirement, you can add other option and modify the post as shown in above comment(//).

Thanks, 

[j.floyd.fusion360]

When I search this, I get that first line of code the

function onCycle() {

but nothing else matches.

I am using a FANUC generic post and it seems whenever deep drilling is selected it enables the G98 instead of G99 for feed.

I used the first part you mentioned to fix the G98 section, but I also have a full IPM given on the posted code.

What more do you need from me to help fix this?

[KrupalVala]

Hi @j.floyd.fusion360 ,

In you case, You need to change G98 to G99 manually And to get IPR/MPR instead of IPM/MPM, set useG95: true, in the post properties.

thanks,  

[KrupalVala]

Hi @j.floyd.fusion360 ,

Please consider this solution if you are using Fanuc Turning post,

Open your post in any editor. Search below code and change the if condition as shown below,

gFeedModeModal.reset();
 //if (currentSection.feedMode == FEED_PER_REVOLUTION) { 
 if (currentSection.feedMode == 0 && getParameter("operation-strategy") == "drill") {
    writeBlock(getCode("FEED_MODE_UNIT_REV"));
  } else {
    writeBlock(getCode("FEED_MODE_UNIT_MIN"));
  }

Now Define var F as shown below,

if (isFirstCyclePoint()) {
    repositionToCycleClearance(cycle, x, y, z);

    //var F = cycle.feedrate;
    var F = (gFeedModeModal.getCurrent() == 99 ? cycle.feedrate/spindleSpeed : cycle.feedrate);
    var P = !cycle.dwell ? 0 : clamp(1, cycle.dwell * 1000, 99999999); // in milliseconds

 and For the case of Tapping add If condition,

case "tapping":
      if (!F) {
        F = tool.getTappingFeedrate();
      }
      // F = tool.getThreadPitch() * rpmFormat.getResultingValue(spindleSpeed);
      if (properties.useRigidTapping != "no") {
        startSpindle(true, false);
      }

Now save the post and test the code carefully. It will give you a desired NC output.

Thanks,

[KrupalVala]

Hi @j.floyd.fusion360  && @Anonymous ,

One correction in the below Code,

if (currentSection.feedMode == FEED_PER_REVOLUTION || getParameter("operation-strategy") == "drill") {

It will give you G99 With Feed Per Revolution in a Drilling as well as Turning Operation.

Thanks, 

[j.floyd.fusion360]

This solves almost all the problem.

Now everything has G99 except grooving cycles.

Those still populate a G98.

What may I do to fix this?

[KrupalVala]

Hi @j.floyd.fusion360 ,

You need to select use feed Per revolution in Toolpath.

thanks,

[j.floyd.fusion360]

Aaah Yes, Simple overlooked mistake. Thank you.