Need post to change G98 to G99 during drilling cycle

[Anonymous]

Hello,

I am trying to set up a post to run on a 2 axis Doosan lathe with milling "C" mode we have. The problem I am having is the code is posting out as a G98 during drilling cycle where as I would like it to be G99 IPR. Have tried several "fixes" that are posted around the web but so far no luck? Could someone help? I attach here my post. 

[KrupalVala]

Hi @Anonymous ,

As you already know how to modified/Set-up the post, please have a look at this form post. 

I hope this helps, but please let me know if you need anything else or if you have any questions.

Thanks,

[iporter6]

my doosan lynx file as requested in your pm.  Let me know if you manage to get feed per rev.

[Anonymous]

Hi @KrupalVala 

I have followed the thread you referenced but the code to search for was not found in mine. I am still trying to force G99 Inches Per Revolution mode automatically during drilling. 

[Anonymous]

Pretty sure it needs a change here, but no luck yet.

[daniel_lyall]

Do a search through the post with G98 and change them as you go to G99

[KrupalVala]

Hi @Anonymous ,

Please search below codes and update as shown below,

// Get active feedrate mode
  if (insertToolCall) {
    gFeedModeModal.reset();
  }
  var feedMode;
  //if ((currentSection.feedMode == FEED_PER_REVOLUTION) || tapping) {
    if (currentSection.feedMode == 0 && getParameter("operation-strategy") == "drill") {
    feedMode = gFeedModeModal.format(getCode("FEED_MODE_MM_REV", getSpindle(TOOL)));
  } else {
    feedMode = gFeedModeModal.format(getCode("FEED_MODE_MM_MIN", getSpindle(TOOL)));
  }

It will give you G99 and IPR value.

Thanks,

[Anonymous]

@KrupalVala 

Ok we are getting closer..... The changes you suggested did change to G99 value but the feedrate is still too fast. Attached are my tool settings, why is it not calculated in program correctly at .003 feedrate?

Thank you for your help!

[KrupalVala]

Hi @Anonymous ,

Please change the unit while Post Processing the NC codes.

Thanks,

[Anonymous]

@KrupalVala 

Yes I have changed to unit, post remains the same. It is inserting the feedrate during cut as the plunge feedrate?

[KrupalVala]

Hi @Anonymous ,

It should work fine.

Please share you CAM project and latest modified if possible. I will check and let you know.

Thanks,

[zwelsh91]

Generally speaking a drilling cycle is a canned cycle. G98 and G99 define the retraction plane Initial or R plane retraction respectively. Understandably on a lathe you would like to use IPR for feedrate. In a standard drilling cycle G81 for example the spindle speed (SFM) is set and the software calculates the feed rate based on your desired IPR in the settings. Feed only really changes on a lathe when you change spindle speed and have IPR feed turned on. So in closing have you tried to use a standard canned cycle like: "Drilling-Rapid Out G81" or "Deep Drilling-Full Retract G83"?

[zwelsh91]

Here is an example of a standard canned drilling cycle for my Daewoo Puma 8S:

(DRILL FOR 3/4-10)
N120 T1010
(.656 DIA DRILL)
G54
/M8
G98
G97 S750 M3
G0 X0. Z2.87
G18
G0 Z2.47
G98 G83 Z0.0229 R0.1 F5.
G80
Z2.87
M9
G28 U0
G28 W0
M1

[Anonymous]

@KrupalVala 

Here is my latest.....Now the drill is correct in G99 mode, but wrong feedrate. But also now turning tools all come in G98 mode! No good...

[KrupalVala · Accepted solution]

HI @Anonymous ,

In a general case, While using a Metric unit Customer Ask for In/min only in the Drilling operation.

But in your case, You already using Imperial/Inch unit and getting In/min in the drilling cycle. Now want to call FEED PER REVOLUTION in Drilling with G99 , You Simply need to change the codes

    if (currentSection.feedMode == FEED_PER_REVOLUTION || getParameter("operation-strategy") == "drill") {
    feedMode = gFeedModeModal.format(getCode("FEED_MODE_MM_REV", getSpindle(TOOL)));
  } else {
    feedMode = gFeedModeModal.format(getCode("FEED_MODE_MM_MIN", getSpindle(TOOL)));
  }

Save the post and test it carefully.

Thanks,

[Anonymous]

@KrupalVala 

Thanks, its working properly now!

[iporter6 · Accepted solution]

@Anonymous does this work for a "non live drill" drilling on centre with the main spindle?  

thanks

[Anonymous]

Yes it is working like you ask. The only problem I can see is it will insert federate given in plunge federate so I just change that manually. I am willing to live with it for now