Clearance in linking param NOT Working

[crazy^millman]

I have answered your question problem is you do not like my answer. Have a great weekend.

[Rstewart]

I have answered your question problem is you do not like my answer. Have a great weekend.

I totally get it and I really appreciate Collin's fix that I hope I can implement.   I just hate it for new mastercam users that may get Bit by this....  

I think CNC should make this standard in their MPMaster post.  Sorry this thread got outta control guys.

[gcode]

I totally get it and I really appreciate Collin's fix that I hope I can implement.   I just hate it for new mastercam users that may get Bit by this....  

I think CNC should make this standard in their MPMaster post.  Sorry this thread got outta control guys.

 

CNC Software has nothing to do with MPMaster posts.

They are a production of InHouse Solutions, the people who provide us with this website.

 

note this line in the X8 Revision Log

 

# IHS 01/13/14  -  Added support for single drill point using clearance at start/end of op only

[Sticky]

I have answered your question problem is you do not like my answer. Have a great weekend.

 

No Ron, you didn't answer ANY of the specific questions I asked. I know you don't like me, if you don't want to answer my questions or add anything valuable to the thread that is ok. Just call me a poopy head or a mastercam hater and move on.

 

I totally get it and I really appreciate Collin's fix that I hope I can implement.   I just hate it for new mastercam users that may get Bit by this....  

I think CNC should make this standard in their MPMaster post.  Sorry this thread got outta control guys.

 

This happens with other non Mpmaster posts too. MPmaster is an InHouse thing, but they ARE aware of this bug and they can modify the post for you.

 

I wouldn't say this thread got out of hand at all. Look how many people didn't know about this problem or how G98 and G99 work. I'd say it is pretty informative.

 

CNC Software has nothing to do with MPMaster posts.

They are a production of InHouse Solutions, the people who provide us with this website.

 

note this line in the X8 Revision Log

 

# IHS 01/13/14  -  Added support for single drill point using clearance at start/end of op only

 

Nice, thanks for the update Gcode.

[crazy^millman]

No Ron, you didn't answer ANY of the specific questions I asked. I know you don't like me, if you don't want to answer my questions or add anything valuable to the thread that is ok. Just call me a poopy head or a mastercam hater and move on.

 

 

 

This happens with other non Mpmaster posts too. MPmaster is an InHouse thing, but they ARE aware of this bug and they can modify the post for you.

 

I wouldn't say this thread got out of hand at all. Look how many people didn't know about this problem or how G98 and G99 work. I'd say it is pretty informative.

 

 

 

Nice, thanks for the update Gcode.

Nope I have respect for you. Yet again I cannot figure out why people who have never meet me in person sure seem to know all about me. I just try to help as best I can and will just bow out. Like I said have a great weekend.

[BenK]

Sticky, if your convinced its a bug don't hesitate to send it in to [email protected]. In the mean time try using a reference point for your retract move, it will force a Z output after your drill operation avoiding this issue.

[Sticky]

Sticky, if your convinced its a bug don't hesitate to send it in to [email protected]. In the mean time try using a reference point for your retract move, it will force a Z output after your drill operation avoiding this issue.

 

Hey Ben, already did that, they already know about it. I used Colin's fix in my post, so I don't have to deal with this anymore, which is awesome. Thanks Colin!

 

But this can still bite someone quite easily is they don't know about it, just like the OP.

 

I first discovered the bug while being on the wrong side of a tombstone on my hmc. I had already drilled a few other holes in G99 on that side and my clearance planes were working as I had set them in MC. Only when I went to either tap or chamfer one hole did I almost send my spindle through the tombstone because it did NOT use the clearance plane on the way out, only on the way in.

 

It is a bug.

 

Notice how not one person has been able to come up with ANY sort of reason on why this works for 2 or more drill points but not 1?

[BenK]

I'm not trying to get in the middle of the argument, just trying to offer a solution to the problem. Honestly I have never seen the issue either on a Fanuc controlled machine so I would talk to an Applications Engineer with the machine builder. But I wanted to stay out of that conversation. 

[gcode]

OK

one more time... this is not a bug.

I created a simple drilling file using Mastercam's generic 3X Haas post.

 

One point posts this

 

 

(T23|3/8 SPOTDRILL|H23|D23|TOOL DIA. - .375)
N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T23 M6
N130 G0 G90 G54 X.2593 Y.1556 S4074 M3
N140 G43 H23 Z2.
N150 G98 G81 Z-.1 R.1 F65.2  <----------------------- Note... G98 even though I enabled G99   ... G99 is not a valid code for 1 hole
N160 G80                                  <------------------------This is valid Fanuc code The spindle WILL return to Z2.0... becauce G98 ... try it an see !!! 
N170 M5
N180 G91 G28 Z0.
N190 G28 X0. Y0.
N200 M30
%

 

Whether  "Use Clearance only at start and end"  is checked or not you get a G98

That's because G99 can't be done, there isn't a second point to stay down and rapid to.

The machine will accept a G99 for one point, but it can't do it.

 

next

 

I pick 3 holes and enable G98

The generic Mastercam post outputs this

 

(T23|3/8 SPOTDRILL|H23|D23|TOOL DIA. - .375)
N100 G20
N110 G0 G17 G40 G49 G80 G90
(3 HOLES  .. G98 ENABLED)
N120 T23 M6
N130 G0 G90 G54 X.2593 Y.1556 S4074 M3
N140 G43 H23 Z2.
N150 G98 G81 Z-.1 R.1 F65.2                               <---------------- correctly outputs G98
N160 X.8815 Y.7037
N170 X1.9333 Y1.2074
N180 G80                                                                <---------------- no return to Z2.  this is valid Fanuc code
N190 M5
N200 G91 G28 Z0.
N210 G28 X0. Y0.
N220 M30
%

 

and finally,  3 points with G99 enabled

 

 

(T23|3/8 SPOTDRILL|H23|D23|TOOL DIA. - .375)
N100 G20
N110 G0 G17 G40 G49 G80 G90
(3 HOLES  .. G98 ENABLED)
N120 T23 M6
N130 G0 G90 G54 X.2593 Y.1556 S4074 M3
N140 G43 H23 Z2.
N150 Z.1
N160 G99 G81 Z-.1 R.1 F65.2   <---------------------------- G99 as requested
N170 X.8815 Y.7037
N180 X1.9333 Y1.2074
N190 G80
N200 Z2.                                     <---------------------------- Output to Clearance plane is output because it is needed
N210 M5
N220 G91 G28 Z0.
N230 G28 X0. Y0.
N240 M30
%

 

In all 3 examples, Mastercam is outputting Fanuc compliant code.

 

I've attached the X8 file I used for this experiment

G99 vs G98.zip

[Guest MTB Technical Services]

G-Code is correct.

 

One slight nuance.

G99 is valid for a single hole canned cycle meaning that it will not generate an alarm.

The only issue is that the built-in Control retract at the end of the cycle is the R-Plane value.

That is the same regardless of the number of positions within the cycle.

An FYI, On any FANUC control, G00 will also cancel any canned drilling cycle.

A G80 isn't required but it's still good practice to use it.

 

For safety purposes, I always have the post output an explicit rapid move in Z to the clearance after cancelling the cycle with G80, regardless of the G98/G99 or the number of hole locations.

 

The issue is really a Post-Processor issue.

It's up to the programmer to enter the proper clearance when plane and angle indexes are required.

It is not a Mastercam software bug.

[Newbeeee™]

 

An FYI, On any FANUC control, G00 will also cancel any canned drilling cycle.

A G80 isn't required but it's still good practice to use it.

 

I didn't know that - everyday's a school day

 

FWIW, all of our rotary vice/fixture work is programmed with a separate work offset per face. Then we can have a separate Z zero as top of stock (each face). So we're then dealing with 'easy to calculate' retracts - ie 5mm retract will clear as it is a value from the Z zero face.

Then for an index move we use a reference point (could be both a Z and an X move - our post outputs Zup followed by the X - no dogleg).

This has worked better for us than using centreline of rotation, because with centre of rotation, you have to then know your clearances for the retracts which could be a bum (large) figure.

Whether this the right way or not...but we started doing it this way after reading a load of posts on here. 

[Sticky]

OK

one more time... this is not a bug.

I created a simple drilling file using Mastercam's generic 3X Haas post.

 

One point posts this

 

 

(T23|3/8 SPOTDRILL|H23|D23|TOOL DIA. - .375)

N100 G20

N110 G0 G17 G40 G49 G80 G90

N120 T23 M6

N130 G0 G90 G54 X.2593 Y.1556 S4074 M3

N140 G43 H23 Z2.

N150 G98 G81 Z-.1 R.1 F65.2  <----------------------- Note... G98 even though I enabled G99   ... G99 is not a valid code for 1 hole

N160 G80                                  <------------------------This is valid Fanuc code The spindle WILL return to Z2.0... becauce G98 ... try it an see !!! 

N170 M5

N180 G91 G28 Z0.

N190 G28 X0. Y0.

N200 M30

%

 

Whether  "Use Clearance only at start and end"  is checked or not you get a G98

That's because G99 can't be done, there isn't a second point to stay down and rapid to.

The machine will accept a G99 for one point, but it can't do it.

 

next

 

I pick 3 holes and enable G98

The generic Mastercam post outputs this

 

(T23|3/8 SPOTDRILL|H23|D23|TOOL DIA. - .375)

N100 G20

N110 G0 G17 G40 G49 G80 G90

(3 HOLES  .. G98 ENABLED)

N120 T23 M6

N130 G0 G90 G54 X.2593 Y.1556 S4074 M3

N140 G43 H23 Z2.

N150 G98 G81 Z-.1 R.1 F65.2                               <---------------- correctly outputs G98

N160 X.8815 Y.7037

N170 X1.9333 Y1.2074

N180 G80                                                                <---------------- no return to Z2.  this is valid Fanuc code

N190 M5

N200 G91 G28 Z0.

N210 G28 X0. Y0.

N220 M30

%

 

and finally,  3 points with G99 enabled

 

 

(T23|3/8 SPOTDRILL|H23|D23|TOOL DIA. - .375)

N100 G20

N110 G0 G17 G40 G49 G80 G90

(3 HOLES  .. G98 ENABLED)

N120 T23 M6

N130 G0 G90 G54 X.2593 Y.1556 S4074 M3

N140 G43 H23 Z2.

N150 Z.1

N160 G99 G81 Z-.1 R.1 F65.2   <---------------------------- G99 as requested

N170 X.8815 Y.7037

N180 X1.9333 Y1.2074

N190 G80

N200 Z2.                                     <---------------------------- Output to Clearance plane is output because it is needed

N210 M5

N220 G91 G28 Z0.

N230 G28 X0. Y0.

N240 M30

%

 

In all 3 examples, Mastercam is outputting Fanuc compliant code.

 

I've attached the X8 file I used for this experiment

 

Hey G, just tried this with Generic 3x and 4x, you are right, it will not post G99 for one hole. Switch to MPMASTER and it WILL post G99 for one hole, which is fine, nothing wrong with that and it works on all Fanuc, Yasnac, Mazak and Haas controls. The PROBLEM is that it won't post the "clearance" value after G80. But it does it for all hole counts over 1.

 

This was so clearly gone over in the thread I linked to earlier, here it is again:

http://www.emastercam.com/board/topic/77464-hmc-programming-training/page-2

 

Page 2, post #32.

 

Your example does not prove that MC doesn't have the bug, only that it won't post G99 with a certain control definition and post.

 

Have you gone out to the floor to test your G99 theory yet G?

 

G-Code is correct.

 

One slight nuance.

G99 is valid for a single hole canned cycle meaning that it will not generate an alarm.

The only issue is that the built-in Control retract at the end of the cycle is the R-Plane value.

That is the same regardless of the number of positions within the cycle.

An FYI, On any FANUC control, G00 will also cancel any canned drilling cycle.

A G80 isn't required but it's still good practice to use it.

 

For safety purposes, I always have the post output an explicit rapid move in Z to the clearance after cancelling the cycle with G80, regardless of the G98/G99 or the number of hole locations.

 

The issue is really a Post-Processor issue.

It's up to the programmer to enter the proper clearance when plane and angle indexes are required.

It is not a Mastercam software bug.

 

Tim, I think you probably know the answer to this, and it seems to be a stumbling block for actually pretty much everyone in this thread, Can you explain what happens when you are drilling in a G99 canned cycle and you call G80?

IE

 

G00 G17 G90 G54 X.75 Y1. S1100 M03

G43 H62 Z5.

G99 G81 Z-1. R.3 F4.11

G80

 

Where is the Z sitting at G80?

 

I don't think this is a post processor issue (but I'm willing to be proven wrong). G's example post won't let you use G99 for one hole, and while that might be the safe way to roll it doesn't prove the status of the NCI data.

 

With the MpMaster posts G99 works correctly for anything over one hole, it WILL use Mastercams "clearance" value after G80. But if you do just one hole it does not post the "clearance" value after G80. Crash time/

[Guest MTB Technical Services]

Hey G, just tried this with Generic 3x and 4x, you are right, it will not post G99 for one hole. Switch to MPMASTER and it WILL post G99 for one hole, which is fine, nothing wrong with that and it works on all Fanuc, Yasnac, Mazak and Haas controls. The PROBLEM is that it won't post the "clearance" value after G80. But it does it for all hole counts over 1.

 

This was so clearly gone over in the thread I linked to earlier, here it is again:

http://www.emastercam.com/board/topic/77464-hmc-programming-training/page-2

 

Page 2, post #32.

 

Your example does not prove that MC doesn't have the bug, only that it won't post G99 with a certain control definition and post.

 

Have you gone out to the floor to test your G99 theory yet G?

 

 

Tim, I think you probably know the answer to this, and it seems to be a stumbling block for actually pretty much everyone in this thread, Can you explain what happens when you are drilling in a G99 canned cycle and you call G80?

IE

 

G00 G17 G90 G54 X.75 Y1. S1100 M03

G43 H62 Z5.

G99 G81 Z-1. R.3 F4.11

G80

 

Where is the Z sitting at G80?

 

I don't think this is a post processor issue (but I'm willing to be proven wrong). G's example post won't let you use G99 for one hole, and while that might be the safe way to roll it doesn't prove the status of the NCI data.

 

With the MpMaster posts G99 works correctly for anything over one hole, it WILL use Mastercams "clearance" value after G80. But if you do just one hole it does not post the "clearance" value after G80. Crash time/

 

I already answered this.

For the sake of clarity, with G99 it will be sitting at R.3 regardless of how many holes are drilled.

Since the issue only occurs with MPMaster posts, this is an In-House Post issue.

[Sticky]

Well hey that at least makes 2 of us!

[Sticky]

Since the issue only occurs with MPMaster posts, this is an In-House Post issue.

 

I don't think the issue is that simple, just because one post doesn't have the function AT ALL and the other does, doesn't mean the problem isn't with the software.

 

If you read the link I posted above, Collin mentions this is an issue with the NCI, not the post. Being that he used to write posts for cnc software he is probably right.

[Guest MTB Technical Services]

I don't think the issue is that simple, just because one post doesn't have the function AT ALL and the other does, doesn't mean the problem isn't with the software.

 

If you read the link I posted above, Collin mentions this is an issue with the NCI, not the post. Being that he used to write posts for cnc software he is probably right.

 

Colin knows the posts and the NCI so I'll take his word as gospel.

It sounds as if CNC has had their posts modified to cover it.

If it's a known NCI issue, don't hold your breath waiting for it to be fixed if a post mod will do it.

[Sticky]

Colin knows the posts and the NCI so I'll take his word as gospel.

It sounds as if CNC has had their posts modified to cover it.

If it's a known NCI issue, don't hold your breath waiting for it to be fixed if a post mod will do it.

 

 

Exactly

[gcode]

I just tried this in X5MU1, the earliest X version I have installed on this machine and got the same results that I got in X8

 

 

(NC FILE - C:\DOCUMENTS AND SETTINGS\******* \MY DOCUMENTS\MY MCAMX5\MILL\NC\T.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T6 | 1.0 X 120 DEGREE SPOT DRILL 3" OUT OF HOLDER | H6 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( SPOT CHECK 1.062" DIA HOLES )
N104 T6 M6
N106 G0 G90 G54 X.1989 Y.4282 S650 M3
N108 G43 H6 Z2.
N110 Z.1
N112 G99 G81 Z-.1 R.1 F3.
N114 X.4822 Y.6103
N116 X.7553 Y.7688
N118 G80
N120 Z2.
N122 M5
N124 G91 G28 Z0.
N126 G28 X0. Y0.
N128 M30
%
 

[slyym]

Wow this is still going?????

[Sticky]

I just tried this in X5MU1, the earliest X version I have installed on this machine and got the same results that I got in X8

 

 

(NC FILE - C:\DOCUMENTS AND SETTINGS\******* \MY DOCUMENTS\MY MCAMX5\MILL\NC\T.NC)

(MATERIAL - ALUMINUM INCH - 2024)

( T6 | 1.0 X 120 DEGREE SPOT DRILL 3" OUT OF HOLDER | H6 )

N100 G20

N102 G0 G17 G40 G49 G80 G90

( SPOT CHECK 1.062" DIA HOLES )

N104 T6 M6

N106 G0 G90 G54 X.1989 Y.4282 S650 M3

N108 G43 H6 Z2.

N110 Z.1

N112 G99 G81 Z-.1 R.1 F3.

N114 X.4822 Y.6103

N116 X.7553 Y.7688

N118 G80

N120 Z2.

N122 M5

N124 G91 G28 Z0.

N126 G28 X0. Y0.

N128 M30

%

 

 

That is exactly what I get when I do 2 holes too. What happens when you do 1 with an Mpmaster post that hasn't been modified to fix this problem?

 

Wow this is still going?????

 

Do you still think G80 sends the Z to the initial plane?

[gcode]

That is exactly what I get when I do 2 holes too. What happens when you do 1 with an Mpmaster post that hasn't been modified to fix this problem?

 

 

Do you still think G80 sends the Z to the initial plane?

in G98 yes  ALL . DAY . LONG

in G99 no

[Sticky]

Well G80 actually doesn't command motion, the Z is already at whatever position specified by the use of G99 or G98, G80 is cancel only.

 

Regardless, glad to see you agree on where the Z is after G98 or G99 now.

[Guest MTB Technical Services]

Just a point of clarification.

 

G80 simply cancels the modal cycle.

It is G98/G99 that determines the retraction point after the cycle is executed at each location.

The machine positioning mode(rapid traverse vs interpolation) is the modal state immediately prior to the cycle call.

 

I bring this up because not all machines allow a simple angular word change for the next hole.

For this to work it needs to be a full rotary axis and not just an indexing axis.

It the rotary axis is an indexing axis only then the cycle must be cancelled after each angular position and called explicitly for the next.

Keep in min that this is simply the generally accepted practice and there may be rotary indexing machines with Fanuc controls that fully support angular word changes within a cycle.

It's the machine builder that controls implementation of that stuff and it also depends upon the rotary unit interface itself.