Sign in to follow this  
PcRobotic

How do I change words in the DRILL CYCLE?

Recommended Posts

Hello everyone,
   My company has two type of machines HAAS (brand new VF2 SSY) and brand new HARDINGE (FANUC control brand new), they both have PROBE.  I just made the probing system works for both FANUC and HAAS.  I also implemented the Q.C function into the post.  

   My question is, "Is that possible that I can change the words  - APPLY CUSTOM DRILL PARAMETERS to another my own words such as PROBE QC - CMM".  I haved look into the post for the key words "APPLY CUSTOM DRILL PARAMETERS ", I also tried to look into the MACHINE DEFINITION but not found where I can change it. 

Modified.png.72cf065fadcde696c3b41cdbb737d394.png

Please help and thank you.

Share this post


Link to post
Share on other sites

Not that I'm aware of, unless you can hack the DLL's in Mastercam, with something like Resource Hacker. But that isn't a "Post Defined" label, the way the actual Parameter Names are...

  • Like 1
  • Haha 1

Share this post


Link to post
Share on other sites
On 12/12/2019 at 5:54 PM, PcRobotic said:

Hello everyone,
   My company has two type of machines HAAS (brand new VF2 SSY) and brand new HARDINGE (FANUC control brand new), they both have PROBE.  I just made the probing system works for both FANUC and HAAS.  I also implemented the Q.C function into the post.  

   My question is, "Is that possible that I can change the words  - APPLY CUSTOM DRILL PARAMETERS to another my own words such as PROBE QC - CMM".  I haved look into the post for the key words "APPLY CUSTOM DRILL PARAMETERS ", I also tried to look into the MACHINE DEFINITION but not found where I can change it. 

Modified.png.72cf065fadcde696c3b41cdbb737d394.png

Please help and thank you.

It may be possible to inherit the drill toolpath type into a "custom" chook operation then modify those string values, however this would require the c++ public sdk and an example project, you would need to request from CNC software, this would be an immense undertaking for a small gain.. I'm curious why you want to do this?

  • Thanks 1

Share this post


Link to post
Share on other sites
On 12/13/2019 at 3:05 PM, peter ~ said:

It may be possible to inherit the drill toolpath type into a "custom" chook operation then modify those string values, however this would require the c++ public sdk and an example project, you would need to request from CNC software, this would be an immense undertaking for a small gain.. I'm curious why you want to do this?

Hello Peter,
   Thank you for asking.  I am in a company of which the are "OVER LOAD" for Q.C department and I am using HAAS as a QC equipment instead of waiting for days or even weeks.  As you already saw above image, the top portion is to allow the PROGRAMMER to use PROBE as pickup work coordinates. 

 

     On the other hand, if user wanted to, he can demand the machine Q.C after the part is completed.  I am not sure if my idea the greatest and if you have something better, I am very happy to take it from you. 

 

     Of course, I still have to submit to the Q.C department for F.A.I and I use the machine as to ENSURE that parts are intolerance if I run every 5 pieces or even 10 of 500 or 1000.

 

 

I truly appreciate for your help,
   S.Luong 

 

===============================

%
O2854(500280.500354 REVC- OP2.nc)
(SOURCE = 500280.500354  REVC.MCAM)
(POSTED ON DEC.09.2019 AT 15*28PM)
(SLUONG, BY= PCROBOTIC\ADMIN)
(*)
(OFH COPPER, ROUND STOCK= 4.00D .53L)
(NOTE= PRODUCTION)
(*)
(TOTAL TOOLS FOR OP2 = 7 TOOLS)
(T3= .5, 1/2 FLAT ENDMILL, U, 4FLTS * Z-.144)
(T4= .375, 3/8 FLAT ENDMILL, U, 4FLTS * Z-.202)
(T6= .25, 1/4 FLAT ENDMILL, U, 4FLTS * Z-.423)
(T22= .25, 1/4 EM, FIN, 3FLTS CB * Z-.423)
(T28= .1875, 3/16 CHMF, CB * Z-.2833)
(T29= 1., 1 DEBURR BRUSH, COLBALT * Z-.159)
(T31= .236, PROBE * R0.1180, U, 4FLTS CM * Z-.25)
(*)
(WORK OFFSET LIST)
(G57)
(XY0 = CENTER)
(Z0 = TOP)
(*)
(CYCLE TIME = 32M 13.52S)
(*)
N31(PROBE XY CENTER BORE, 1.531, CUT#38)
G0 G17 G40 G49 G80 G90
G91 G28 Z0 M19
G17(XY PLANE) G28 Y0.
T31 M6(.2360,PROBE, U, CERAMIC, 2.000RLF,)
G90 G57 X0. Y0.
G43 H31 Z3. T3(DOC= Z-.25)
G4 P5.(BORE)
G65 P9832 G1 Z3. F25.(PROBE ON)
G65 P9810 G1 Z2. F25.(PROTECTIVE MOVE)
G65 P9810 G1 Z1. F25.
G65 P9810 G1 Z-.25 F25.(APPROACHING)
G65 P9995 W57.(WO#) A10. D1.531(D)
G0 G90 Z3.
G65 P9833(PROBE OFF)
G91 G28 Z0.
G28 Y0. M5
G0 G90 G57 X0.
M1
(*)
N22010(FINISH 1X  3.303, CUT#68)
G0 G17 G40 G49 G80 G90(24.74S)
G91 G28 Z0 M19
G17(XY PLANE) G28 Y0.
M31(CHIP CONVEYOR ON)
T22 M6(.2500,1/4 EM, FIN, CB, 2.000RLF,)
G90 G57 S5000 M3
X1.314 Y-.1252
G43(D22)H22 Z2. T31(DOC= Z-.025)
/G4 P5. M88
G17(XY PLANE) G90 Z.1
G1 Z-.025 F25.
G41 D22 X1.4015 Y-.1253
G3 X1.5265 Y-.0003 R.125
X1.5265 Y-.0003 I-1.5265 J.0003
Y.0097 R1.5265
X1.4007 Y.1339 R.125
G1 G40 X1.3132 Y.1334
G0 Z2.
M89
M33(CHIP CONVEYOR OFF)
G91 G28 Z0.
G28 Y0. M5
G0 G90 G57 X0.
M1
(*)
N3103(QC 3.005 ID, CUT#69)
G0 G17 G40 G49 G80 G90
G91 G28 Z0 M19
G17(XY PLANE) G28 Y0.
T31 M6(.2360,PROBE, U, CERAMIC, 2.000RLF,)
G90 G57 X0. Y0.
G43 H31 Z3. T31(DOC= Z-.25)
G4 P5.(BORE)
G65 P9832 G1 Z3. F25.(PROBE ON)
G65 P9810 G1 Z2. F25.(PROTECTIVE MOVE)
G65 P9810 G1 Z1. F25.
G65 P9810 G1 Z-.25 F25.(APPROACHING)
G65 P9995 W59. A10. D3.005(D)
G0 G90 Z3.
G65 P9833(PROBE OFF)
M0(COMPARE 10188 MACRO - PRINT VALUE)
G91 G28 Z0.
G28 Y0. M5
G0 G90 G57 X0.
M30(184,587 CHARACTERS = 185.19KB)
%
 

Share this post


Link to post
Share on other sites

Oh ok I did not understand the first time

  • Like 1

Share this post


Link to post
Share on other sites

Might better watch using your machines to inspect parts if the machine has not been calibrated. If your audited and the parts are for AS9100 and the machine have not had the proper artifact run on them to insure they are measuring correctly every one of those parts will be considered bad using falsified inspection data putting your company in jeopardy of fines and other things. If not under any kind of a QMS, ISO-9000, ISO-9001 or AS9100 quality requirement and just for sanity checks then okay, but using a machine as a CMM requires very precise method and documentation in your Quality management documentation as well as your training. 

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites
2 hours ago, 5th Axis CGI said:

Might better watch using your machines to inspect parts if the machine has not been calibrated. If your audited and the parts are for AS9100 and the machine have not had the proper artifact run on them to insure they are measuring correctly every one of those parts will be considered bad using falsified inspection data putting your company in jeopardy of fines and other things. If not under any kind of a QMS, ISO-9000, ISO-9001 or AS9100 quality requirement and just for sanity checks then okay, but using a machine as a CMM requires very precise method and documentation in your Quality management documentation as well as your training. 

Hello 5th Axis,
   Every morning I always calibrate my probe with MASTER RING GAUGE and most of the time it is +/-.0002.  I think this should be taken care of.

 

PS:  I also purchased 1mm (.0393) tip to check tiny holes as well.

 

Thank you for the suggestion,
    S.Luong

Share this post


Link to post
Share on other sites
2 hours ago, PcRobotic said:

Hello 5th Axis,
   Every morning I always calibrate my probe with MASTER RING GAUGE and most of the time it is +/-.0002.  I think this should be taken care of.

 

PS:  I also purchased 1mm (.0393) tip to check tiny holes as well.

 

Thank you for the suggestion,
    S.Luong

Hi Steven,

What do you mean by "I think this should be taken care of", in reference to Probe Calibration?

It sounds like you are already "taking care of it", by performing the Calibration of your Probe. When I'm calibrating, I always run the following calibration programs, in order:

  1. Run the 'Tool Probe Calibration' routine first. Use a proper "Calibration Tool" of "known length". I like the ones from Maritool, since they are very inexpensive for a decent quality tool. https://www.maritool.com/Tool-Holders-CAT40-CAT40-Calibration/c23_25_69/p17365/CAT40-Tool-Probe-Calibrator/product_info.html
  2. After qualifying the "Tool Probe", load the Spindle Probe into the machine. Run the 'Spindle Probe Length Calibration' program, from VPS. All you should have to enter is the Tool Number for the Spindle Probe.
  3. Now, run the 'Spindle Probe Diameter Calibration', using a securely mounted Ring Gauge on your machine table. You can sometimes use magnets to hold the gauge, but be careful that there is enough grip force holding the ring gauge, so it doesn't slip when Probing. Renishaw recommends a Ring Gauge Diameter of at least 50 mm (or 2.0 Inches), or bigger. Your calibration will suffer a bit, if your gauge is too small. (* by suffer, I mean maybe .0001-.0002 T.I.R. of difference, maximum.) I recommend a Mitutoyo Ring Gage. https://ecatalog.mitutoyo.com/Setting-Ring-Series-177-Accessories-for-Inside-MicrometersHoltest-and-Dial-Bore-Gages-C1525.aspx I would recommend model 177-293 (2.4" Hole, +-0.00006").

Again, what do you think should be "taken care of"?

Keep these guidelines in mind:

  • You should always perform Calibration on a "warm machine". This means both the Spindle is warm, and the Axis Drive Motors are warm. When I setup a Calibration procedure at a new company, I recommend that they modify their Spindle Warm-up Program, to include X, Y, and Z axis motion. If the Linear Axes are cold, you might get .0001-.0003 growth (+ or -), based on a cold machine, or a warm machine. For my warm-up programs, I'm typically stroking XY first, then returning to a safe position, then stroking Z. While I'm performing the stokes of the linear axes, I'm also going through the 'spindle ramp up', and then 'spindle ramp down'. I would do this for at least 10 minutes, in order to get the best calibration results.
  • A Renishaw OMP 40-2 Probe (standard on the Haas), has mechanical repeat-ability of about +-.00004 Inches. (1 micron = .000039 Inches)
  • A Haas Mill (*when fully warm*), has a mechanical repeat-ability of about .0004. This is just a physical limitation of the machine, control, and mechanical motion feedback loop.

So, the Probe you are using, is about 10x more accurate, than your machine is capable of repeating to.

There is nothing wrong with the Probe or the Control Software. You are just at the physical limits of what a Haas is capable of. The fact that you are getting +-0.0002 on your Probe is simply proving that fact.

If you need better repeat-ability than that; buy a Matsuura!

Hope that helps,

Colin

 

 

 

  • Like 1

Share this post


Link to post
Share on other sites
2 hours ago, PcRobotic said:

Hello 5th Axis,
   Every morning I always calibrate my probe with MASTER RING GAUGE and most of the time it is +/-.0002.  I think this should be taken care of.

 

PS:  I also purchased 1mm (.0393) tip to check tiny holes as well.

 

Thank you for the suggestion,
    S.Luong

So then all your ever checking is holes then great in that same exact position? CMM Calibration is not verifying it can check the part accurate in one place repeatable, but in all places repeatably. There is a complete volumetric process a CMM goes through according to ISO 10660 that allows the people putting the sticker on your CMM must follow. By what your doing your only ensuring that the probe can measure a round feature and again if that is all your checking with the machine then your good. However if your checking for true position, parallelism, perpendicularity, flatness, and other GD&T features without checking an Artifact that has been verified by and outside NIST or ISO certified lab with results to compare them to then your company is not doing or going about it correctly. 

Share this post


Link to post
Share on other sites

Hi Steven,

There is also something you should be aware of:

  • The Calibration and Measurement cycles on the Haas are all designed to be used together. This is the default package of Macros that come "from the factory" on Haas machines.
  • All of the Renishaw packages have Macro programs which are interrelated. This means that you should not try and modify the Macro programs directly, in most circumstances. 
  • There are a few programs that you should know about and know how to edit. One of those is the 'settings' Macro program. I believe this is something like 9837, or something like that. When you look in the '9000' program folder on the machine (NGC), you'll see comments and program numbers. One of the comments should be 'Renishaw settings'. This allows you to modify things like "probing fast Feedrate inch" values.
  • The default Macros only store and load, a single set of Probing Parameter Values. These values (variables) are stored during the Calibration process. 
  • Renishaw has other packages of Probing Macros available (for purchase), which allow you to do things like "record different 'sets' of Calibration Variables, for different Probe Feedrate values, and different Probe Tip Diameters.
  • It is important to note that in order for you to Probe features at different Feedrate speeds, you would have to (with the Haas Default Probe Package), modify the Settings Macro, Recalibrate with the new values, and then Probe your part. Then, when you want to Probe at a different speed, you would repeat the process of modifying the Calibration program, Recalibrating the Probe (stores probe variables), and probing a new feature. 
  • The more advanced packages for Probing allow you to calibrate and store at least a couple different Probe Tip and Parameter values. Then, you can call a 'load probe values' macro, and pass a variable to tell the Macro "load a specific set of values". You can call this on-the-fly, just before you measure. 
  • Why would you want to Probe at different speeds? Probing accuracy is inherently based on the speed that the measurement is taken at. By default, I think the '2nd hit speed' is 2.0 inches per minute. (50mm /min). To get maximum accuracy from the Probe, you must Probe that slowly. But what if you only need a rough location for setting a Work Offset, from a saw-cut end of the stock? You could probe at 50 inches per minute, and still get about +-.001-.0015, depending on the machine, and that might be good enough for that operation.
  • What you can't have; is both fast speed, and accurate measurements. There is always a give-and-take between the two parameters. So a compromise must be made somewhere. The Haas Probing package is setup to work out-of-the-box, with a minimum of fuss by the operator.
  • There are some Macros which are included in the Control, but for which there are not any 'VPS Templates' for. The Feature-to-Feature measuring Macro, is one of those. To use it, is a multi-step programming process. You have to 'measure feature 1', run the F2F Macro with no-arguments (variables) being passed. Then you 'measure feature 2'. Then you need to immediately run the F2F macro a 2nd time, but you must enter Parameters which tell the Macro, which direction are you measuring and what type of feature is it?

Share this post


Link to post
Share on other sites

Question from a non-Haas guy about Haas; when calibrating the OMP's length, do you use the Tool Measurement system to do it?

Share this post


Link to post
Share on other sites
On 12/19/2019 at 10:00 AM, cncappsjames said:

Question from a non-Haas guy about Haas; when calibrating the OMP's length, do you use the Tool Measurement system to do it?

I have bought the holder of which has the KNOWN LENGTH and the PRECISED DIAMETER as well.  Not sure the best way but please teach me how if you have better idea.

 

 

Thank you.

  • Like 1

Share this post


Link to post
Share on other sites

All this machining center talk makes me jelly working with routers makes me miss the knitty gritty of metal shop.

Share this post


Link to post
Share on other sites

As someone has already mentioned:

Please note: That I don't advice on editing of any of Mastercam files as it will void your user software agreement!

drill.png

  • Like 1

Share this post


Link to post
Share on other sites
On 12/20/2019 at 1:32 PM, PcRobotic said:

I have bought the holder of which has the KNOWN LENGTH and the PRECISE DIAMETER as well.  Not sure the best way but please teach me how if you have better idea.

Thank you.

I don't know that my way is the "best" way, and I'm sure there's a faster way but it gets me to within .0001 or better every time; 

  1. Using a tape measure or scale, I estimate the length of the probe (to the tip) and add a "little" :) and put that value in the probe's length geometry offset. 
  2.  Taking your known length tool, set your G54 (or an open offset) to the top of a FLAT easily accessible surface. I use a 4" gage block so I dont move Z and compress the bearings, and I can make my offset good wo within .0001"
  3. Call your probe into the spindle. 
  4. Activate G54 (or the work offset  you used)
  5. "Measure" that Z surface you set your work offset to with a probing cycle. No S value on the probe cycle line. Whatever you do, DO NOT reset that surface as your Work Offset Z Zero or you need to go back to step 2.  
  6. Once you "measure" that surface, you will have an "error" value in one of them. Not being a Haas guy I don;t know what your variables are (on a FANUC it would be #142).
  7. Put that error value in your probe's length offset "WEAR" column.
  8. Measure again. The error should be 0 or maybe .0001" or so.
  9. If that was the case, add the value in your wear column to your geometry column and clear the WEAR offset. 
  10. Measure one more time. The error should be within .0001" of what it was in the previous measure's error. 

Again, not saying my way is the best way, this is just the most foolproof way I figured out BITD when I was learning.

The reason I do not use the tool measurement system to set probe length offsets is because 1) If it is touch style tool measurement system, you will get the probe's length without taking into account the deflection/trigger point in Z so measurements would be a little off.  2)If the measurement system is laser, there's virtually no chance of getting a good offset because spinning the probe at normal tool measurement RPM's will destroy a probe or the ruby will deflect the laser beam and give an erroneous measurement. 

Hope this helps.  

  • Like 1

Share this post


Link to post
Share on other sites
7 hours ago, cncappsjames said:

I don't know that my way is the "best" way, and I'm sure there's a faster way but it gets me to within .0001 or better every time; 

  1. Using a tape measure or scale, I estimate the length of the probe (to the tip) and add a "little" :) and put that value in the probe's length geometry offset. 
  2.  Taking your known length tool, set your G54 (or an open offset) to the top of a FLAT easily accessible surface. I use a 4" gage block so I dont move Z and compress the bearings, and I can make my offset good wo within .0001"
  3. Call your probe into the spindle. 
  4. Activate G54 (or the work offset  you used)
  5. "Measure" that Z surface you set your work offset to with a probing cycle. No S value on the probe cycle line. Whatever you do, DO NOT reset that surface as your Work Offset Z Zero or you need to go back to step 2.  
  6. Once you "measure" that surface, you will have an "error" value in one of them. Not being a Haas guy I don;t know what your variables are (on a FANUC it would be #142).
  7. Put that error value in your probe's length offset "WEAR" column.
  8. Measure again. The error should be 0 or maybe .0001" or so.
  9. If that was the case, add the value in your wear column to your geometry column and clear the WEAR offset. 
  10. Measure one more time. The error should be within .0001" of what it was in the previous measure's error. 

Again, not saying my way is the best way, this is just the most foolproof way I figured out BITD when I was learning.

The reason I do not use the tool measurement system to set probe length offsets is because 1) If it is touch style tool measurement system, you will get the probe's length without taking into account the deflection/trigger point in Z so measurements would be a little off.  2)If the measurement system is laser, there's virtually no chance of getting a good offset because spinning the probe at normal tool measurement RPM's will destroy a probe or the ruby will deflect the laser beam and give an erroneous measurement. 

Hope this helps.  

My process was much the same, with a slight modification. 

I would calibrate the laser, the measure a new tool in a good holder.  With the measured tool I would then cut a flat on a sacrificial block of material, set the datum, and calibrate the probe on the newly machined flat. 

This process made sure that to tool setter and the probe agreed.   

  • Like 1

Share this post


Link to post
Share on other sites
On 12/19/2019 at 1:00 PM, cncappsjames said:

Question from a non-Haas guy about Haas; when calibrating the OMP's length, do you use the Tool Measurement system to do it?

I made a program to take the 19700 parameters and add them to set work offset to the table face. (We use it to set WCS for camplete also)

 

Then the probe calibration program touches the table and sets probe height.

Share this post


Link to post
Share on other sites
On 12/18/2019 at 1:56 PM, Colin Gilchrist said:

Hi Steven,

What do you mean by "I think this should be taken care of", in reference to Probe Calibration?

It sounds like you are already "taking care of it", by performing the Calibration of your Probe. When I'm calibrating, I always run the following calibration programs, in order:

  1. Run the 'Tool Probe Calibration' routine first. Use a proper "Calibration Tool" of "known length". I like the ones from Maritool, since they are very inexpensive for a decent quality tool. https://www.maritool.com/Tool-Holders-CAT40-CAT40-Calibration/c23_25_69/p17365/CAT40-Tool-Probe-Calibrator/product_info.html
  2. After qualifying the "Tool Probe", load the Spindle Probe into the machine. Run the 'Spindle Probe Length Calibration' program, from VPS. All you should have to enter is the Tool Number for the Spindle Probe.
  3. Now, run the 'Spindle Probe Diameter Calibration', using a securely mounted Ring Gauge on your machine table. You can sometimes use magnets to hold the gauge, but be careful that there is enough grip force holding the ring gauge, so it doesn't slip when Probing. Renishaw recommends a Ring Gauge Diameter of at least 50 mm (or 2.0 Inches), or bigger. Your calibration will suffer a bit, if your gauge is too small. (* by suffer, I mean maybe .0001-.0002 T.I.R. of difference, maximum.) I recommend a Mitutoyo Ring Gage. https://ecatalog.mitutoyo.com/Setting-Ring-Series-177-Accessories-for-Inside-MicrometersHoltest-and-Dial-Bore-Gages-C1525.aspx I would recommend model 177-293 (2.4" Hole, +-0.00006").

Again, what do you think should be "taken care of"?

Keep these guidelines in mind:

  • You should always perform Calibration on a "warm machine". This means both the Spindle is warm, and the Axis Drive Motors are warm. When I setup a Calibration procedure at a new company, I recommend that they modify their Spindle Warm-up Program, to include X, Y, and Z axis motion. If the Linear Axes are cold, you might get .0001-.0003 growth (+ or -), based on a cold machine, or a warm machine. For my warm-up programs, I'm typically stroking XY first, then returning to a safe position, then stroking Z. While I'm performing the stokes of the linear axes, I'm also going through the 'spindle ramp up', and then 'spindle ramp down'. I would do this for at least 10 minutes, in order to get the best calibration results.
  • A Renishaw OMP 40-2 Probe (standard on the Haas), has mechanical repeat-ability of about +-.00004 Inches. (1 micron = .000039 Inches)
  • A Haas Mill (*when fully warm*), has a mechanical repeat-ability of about .0004. This is just a physical limitation of the machine, control, and mechanical motion feedback loop.

So, the Probe you are using, is about 10x more accurate, than your machine is capable of repeating to.

There is nothing wrong with the Probe or the Control Software. You are just at the physical limits of what a Haas is capable of. The fact that you are getting +-0.0002 on your Probe is simply proving that fact.

If you need better repeat-ability than that; buy a Matsuura!

Hope that helps,

Colin

 

 

 

Thank you for your advice, Colin and Merry Christmas.

Share this post


Link to post
Share on other sites
7 hours ago, PcRobotic said:

Thank you for your advice, Colin and Merry Christmas.

Merry Christmas to you as well Steven! I wish you and your family the very best this Holiday season, and blessings for a prosperous 2020!

  • Thanks 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • 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