Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

How to Post out Cutter Diameter as a Fanuc Variable...


Niezingerly
 Share

Recommended Posts

I want to edit my post to output the Programmed Cutter diameter as a Fanuc Variable.

Have searched in the forum, haven't been able to find an answer.

I am no post writer, but have been given to task to figure this out.

 

 Makino Pro 6 control

Mastercam 2022

MPMaster Post.

 

I'd like to see the output as below:

N1 #101 = 0.1250

 

Thanks for the help...

Link to comment
Share on other sites

fmt  "D#" 4 maz_doff    #Mazak Pallet Tech Diameter offset number #added 02/10/2020
fmt  "H#" 4 maz_hoff    #Mazak Pallet Tech Height offset number   #added 02/10/2020

maz_doff = 51999  #modified 02/10/2020
maz_hoff = 51999  #modified 02/10/2020

 

 

 

pccdia          #Cutter Compensation
      #Force Dxx#
       if prv_cc_pos$ <> cc_pos$ & cc_pos$, prv_maz_doff = c9k  ##modified 02/10/2020
       sccomp
       if cc_pos$, maz_doff                                        #modified 02/10/2020

 

 

Link to comment
Share on other sites
54 minutes ago, Tim Johnson said:

Not enough information.

N1 #101 = 0.1250

Are N1, #101 and 0.1250 each separate variables or is this a hard line that never changes?

If variables, where are the three variables stored for retrieving purposes?

 

I was thinking the same thing, but if dare ask such a question I am just mean. :welcome::rtfm:

  • Haha 1
Link to comment
Share on other sites

Woops...

 

N1 is just there as a generic line number. 

It could always be N1, or just follow the sequence of N numbering that the post does for line numbering.

 

#101 will always wants to be the exact same, every time it is output.  Essentially is could be hard-coded in...

 

0.125 is there to represent the true defined diameter of the cutter in Mastercam.  I just used a generic number to represent it, but, if the defined cutter in Mastercam was 1/4" diameter end mill, then this value would want to be that exact diameter, in decimal output, which would be 0.2500...

 

I am unsure what you are asking, about where the variables would be stored.

What I am trying to achieve is having the exact diameter, from Mastercam, output in the format above into the NC program, and when the NC program with this line is run at the machine, the machine will hit that line, read the info, and set machine variable #101 to whatever numeric value is there...

 

Not sure if the clarifies it, but thank you for the help.

 

Shown below is output I'd like to see...

 

Yellow highlighted is the cutter used in the operation

Green highlighted is what I would like to see output from the post..

 

image.png.da37312038e922612b5717b7cf3f7940.png

Link to comment
Share on other sites
1 minute ago, Niezingerly said:

Woops...

 

N1 is just there as a generic line number. 

It could always be N1, or just follow the sequence of N numbering that the post does for line numbering.

 

#101 will always wants to be the exact same, every time it is output.  Essentially is could be hard-coded in...

 

0.125 is there to represent the true defined diameter of the cutter in Mastercam.  I just used a generic number to represent it, but, if the defined cutter in Mastercam was 1/4" diameter end mill, then this value would want to be that exact diameter, in decimal output, which would be 0.2500...

 

I am unsure what you are asking, about where the variables would be stored.

What I am trying to achieve is having the exact diameter, from Mastercam, output in the format above into the NC program, and when the NC program with this line is run at the machine, the machine will hit that line, read the info, and set machine variable #101 to whatever numeric value is there...

 

Not sure if the clarifies it, but thank you for the help.

 

Shown below is output I'd like to see...

 

Yellow highlighted is the cutter used in the operation

Green highlighted is what I would like to see output from the post..

 

image.png.da37312038e922612b5717b7cf3f7940.png

That is a better way for someone to help thank you for supplying the needed information.

 

Link to comment
Share on other sites

Tool length offset value active (by variable number):

#5081 = GEO

#5082 = GEO WEAR

#5083 = RADIUS

#5084 = RADIUS WEAR

Tool length offset value active (by variable name):

[#_TOFS[1]] = GEO

[#_TOFS[2]] = GEO WEAR

[#_TOFS[3]] = RADIUS

[#_TOFS[4]] = RADIUS WEAR

[#_TOFS[5]] = CORNER RADIUS (if applicable)

[#_TOFS[6]] = CORNER RADIUS WEAR (if applicable)

  • Like 2
Link to comment
Share on other sites

So, I have tried the edits provided from JParis, and I got output that is something close to what I need to see, but...

The first pic below is the edit I made to the post, green highlight is what I ended up putting into the post.

image.png.913d8bc6893de6a198a634a2303176bf.png

 

The 2nd picture is the output I got...Yellow Highlight is the output I got.

image.png.b310c2fea0cfbea52bb2efe647e2a620.png

 

The "D" right before the 0.2362 is the issue.  It needs to not be there.

 

tldia$ looks to be formatted as a note in this post.

image.png.61241b920ce07d5c3891fb7a4c25a8cf.png

 

Again, I am no post writer, but is there a way to create "something else" that will get the cutter diameter from Mastercam, and be useable for what I need?

 

 

As I have been going over this, I am realizing I probably put this in the wrong forum, if so, please let me know and I will tansfer this over to the Post Processor forum...

 

Thanks in advance for the help and thanks for the help so far...

 

 

Link to comment
Share on other sites

What are you doing with the #101 variable? Are you using it for "D#101" when using Cutter Compensation?

I've seen and written plenty of Posts to capture the actual Tool Diameter, but typically I'm buffering that information during the Pre-Read (Tool Table) output, and then writing G10 Lines at the top of the program to overwrite the Tool Diameter Compensation values in the Offsets Table on the machine, so we don't end up with an incorrect Tool Diameter that someone forgot to clear out.

Or are you using it with a Tool Probing Routine to take the "Nominal Tool Diameter" for use in a Probing formula to calculate the difference between nominal diameter and measured diameter?

Link to comment
Share on other sites

I am using it to verify the cutter in the spindle, at the time of cutting, is the correct diameter, to what is programmed in Mastercam.

I plan on "re-lasering" the diameter of the cutter, that was loaded by the program, into the spindle, and then comparing the active cutter diameter with what the Programmed diameter is in Mastercam.

We are having alot of issues where due to us humans being faulty, an incorrect diameter cutter is loaded into the machine, and run with a program that it was not meant for.

Example:

T01 in Mastercam:  0.5mm Sharp End Mill

T01 loaded into the tool changer:  0.8mm Sharp End Mill

(Yeah, I know this shouldn't happen, but it does...)

The machine reads the program, goes and loads T01 into the spindle, and sadly, T01 is bigger than it should be.

Bye bye metal, hello scrapped part.

 

So, I am getting something together to like I said "re-laser" the cutter that has been loaded into the spindle, compare the true cutter from the laser to the Theoretical Cutter diameter that is stored from the program, (which comes directly from Mastercam, HOPEFULLY taking out the human error part of things), and then do a little logic to compare the true cutter diameter to the theoretical cutter diameter, and if it varies more than some certain amount, Alarm time....

 

  • Like 2
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...