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:

Retract?

MetalMarvels

By MetalMarvels,
in Industrial Forum

 Share

Recommended Posts

MetalMarvels Newbie

MetalMarvels

Posted
Posted

This has been puzzling me for awhile now and I am now at a loss as to where to look for the “answer”. My problem is that after each tool completes, it retracts well above the tool changer Z-height then moves back down to the tool changer Z-height and completes the M6 tool change. I am using MC 9.1, a Fadal 3016L, and a modified MPFADAL post (modified to correct some rigid-tap issues and to add the “TA” at the top of the code). This only happens when one or more of the tool lengths are within 2 inches of the top of the part. It happens whether I use the G91 or a G90 (such as in line N120). If I use a large initial plane height (say 2 inches), the retract before the tool change can cause me to run out of Z-travel and cause a subsequent axis error. It is like the Fadal is “looking ahead” and goes to the M6 height and “adds” the tool retract to it. This happens if the previous op was a canned cycle or a regular cycle, but it only happens if a tool (at the tool change Z-height) is within a couple of inches of the top of the part. If the closest tool is farther than about 2 inches, the tools will retract normally to the tool change Z-height.

 

Any thoughts???

 

TA,1

%

N10 O0001 ( 110-50851A FRONT )

(DATE=DD-MM-YY - 23-06-03 TIME=HH:MM - 08:40 )

N20 G20

N30 G0 G17 G40 G49 G70 G80 G90 H0 E0 Z0

N40 ( 3 MM SPOTDRILL TOOL - 7 DIA. OFF. - 7 LEN. - 7 DIA. - .1181 )

N50 ( DRILL )

N60 T7 M6

N70 G0 G90 S6800 M3 E1 X6.94 Y-.313

N80 H7 Z.25 M8.1

N90 G81 G98 Z-.03 R0.01 F6.53

N100 G80

N110 M5 M9

N120 G0 G91 H0 Z0.

N130 M1

N140 ( 7/32 DRILL TOOL - 13 DIA. OFF. - 13 LEN. - 13 DIA. - .21875 )

N150 T13 M6

N160 G0 G90 S4191 M3 E1 X6.94 Y-.313

N170 H13 Z.25 M8.1

N180 G83 G98 Z-.198 R0.01 Q.0656 F8.45

N190 G80

N200 M5 M9

N210 G0 G91 H0 Z0.

N220 M1

Link to comment
Share on other sites
CAM-mando Newbie

CAM-mando

Posted
Posted

Im not a FADAL guy, but my guess is that the H0 is canceling Tool Length Comp, so the Z is required to travel a minimum of the Comp amount to ensure no Z minus movement. With large Comp values it is traveling past Tool Change Plane.

 

We have a machine with tool change position about 1" below Z home and it drives me nuts on tall Work pieces. It does that Z minus hitch before a tool change. eek.gif

Link to comment
Share on other sites
Thad Enthusiast

Thad

Posted
Posted

Is there a value in your E1 for the Z axis?

 

Is your Z cold start position set correctly? To check, from the command line, type in TC,1 ENTER. The control will show you the distance to go to the tool change position. This number should match the Z readout value. If not, your Z needs to be reset.

 

What is your clearance height? If the tool is 1 inch above the part at the tool change position and you tell it to go to Z2. H1, that would force the tool above the tool change position. Just a thought...

 

Thad

Link to comment
Share on other sites
MetalMarvels Newbie

MetalMarvels

Posted
  • Author
Posted

Mayday, I remember that we tried a G28 some time ago and got into some serious trouble (i.e. a new spindle mad.gif ) and didn't go back to it. I suspect it is because we (ok - I) don't really understand what is happening at the controller with the various coordinate systems on the machine.

 

CAMmando,that Z-hitch is exactly the problem.. Doesn't hurt anything unless my tool retract initial plane is too tall.....

 

thad, I definitely have Z offsets in E1. I typically use a tool height probe for all of my tools (that way I can change out a tool in mid-stream) and set my fixture offset as the delta between my tool probe height and the part height. It is usually a positive Z offset in the fixture offset table. The Z-cold start position is at the tool-change Z-height, but I will double check tonight. If it is off - it is certainly not by more than a few tenths.

 

In the example I showed, the tool height above the part is about 1.3 inches at Z-tool change height. The tool clearance is at 0.25 inches above the part with an incremental 0.01 retract height for all tools. The top of stock is set to an absolute value of 0.0 with an absolute depth of -0.03 for the spotdrill.

 

I will experiment further, but perhaps there is some sort of interaction with a positive Z-offset in my fixture offset.......

Link to comment
Share on other sites
cadcam Newbie

cadcam

Posted
Posted

This how I have my post set and works great with the fadal.

 

TA,1

%

O0001 (JAYTESTDRILL REV: )

(JAYTESTDRILL )

(MACHINE TOOL : FADAL FORMAT 1 )

(DATE -23-06-03 )

(TIME -11:19 )

(*)

(MATERIAL: )

(STOCK SIZE: X = 5. Y = 5. Z = 4. )

(HOME POSTION COORIDNATES ARE THE FOLLOWING)

(X= )

(Y= )

(Z= TOP OF PART)

(*)

( TOOL - 10 DIA. - .125 1/8 DRILL )

(*)

(USING FIXTURE OFFSETS: E1 )

(*)

N100 G0 G17 G40 G49 G80 G90

N102 T10 M6 ( TOOL - 10 DIA. - .125 1/8 DRILL )

N104 G0 G90 X.3708 Y3.7747 E1 S5000 M3

N106 G43 H10 Z1. M8

N108 G98 G83 X.3708 Y3.7747 Z-.5 R.25 I.1 J.1 K.1 P.05 F5.76

N110 X.3708 Y4.8567

N112 X4.2671 Y4.8567

N114 X4.2671 Y3.7747

N116 G80

N118 M5

N120 G0 G49 Z0.0 M9

N122 G0 X0. Y0. E0

N124 M0

N126 M2

( BECAUSE YOU HAVE A CHOICE - )

( THANK YOU FOR CHOOSING PRECISION PROGRAMMING )

%

Link to comment
Share on other sites
Dean Lindblad Newbie

Dean Lindblad

Posted
Posted

Gary,

 

In your program the G98 is a "return to initial plane".

 

If the top of your part is at "0" and your initial height is set to

2", but you only have 1" of clearance between your tool and

the part at tool change position, the G98 will send it to the initial

plane while it is still in the canned cycle. Once it comes out of

canned cycle it sees the Z0 H0 and moves it back down

1" to the tool change position. The greater the difference

between your initial height value and your actual tool clearance

the more chance of an axis overtravel error.

 

Hope that makes sense.

 

Dean

Link to comment
Share on other sites
MetalMarvels Newbie

MetalMarvels

Posted
  • Author
Posted

Thanks for all your replies! I think I might have found the problem - the "G91" - I will play with it tonight with no tools in the machine (or parts) and see what I can figure out.

 

N100 G80

N110 M5 M9

N120 G0 G91 H0 Z0.

N130 M1

N140 ( 7/32 DRILL TOOL - 13 DIA. OFF. - 13 LEN. - 13 DIA. - .21875 )

N150 T13 M6

 

According to the Fadal manual, a "G90 G0 H0 Z0" is functionally equivalent to a "G90 G0 G49 Z0" - similar in operation to the code in Jay's example. In my case I have Incremental Positioning (G91) rather than Absolute Positioning (G90) in use. In my case the "H0" acts like a tool length offset cancel - equivalent to the "G49" in Jay's example.

Link to comment
Share on other sites
MetalMarvels Newbie

MetalMarvels

Posted
  • Author
Posted

quote:
Formate 2 and you want incramentl, ok then.

LOL More a case of the Fadal came set up in Format 2, I got a post that mostly worked in Format2, I didn't know any better, and I have been muddling my way through without a complete understanding of everything that goes on interactively in the control. eek.gif

 

I should probably switch to "native" Fadal Format 1 and change the post accordingly. I have started to notice neat little Fadal things that I can't use in Format 2.

 

[ 06-23-2003, 05:48 PM: Message edited by: MetalMarvels ]

Link to comment
Share on other sites
JohnA Newbie

JohnA

Posted
Posted

Make your line before your next tool change look like this:

 

G0 G49 Z0.0

G0 X0. Y0. E0

 

The G49 will cancel your tool length offset and it will use the Z home position as the Z0.0 that it is trying to go to.

Man, did that make any sense at all? I guess I have this thing about putting my thoughts into words, oh well... smile.gif

 

John

Link to comment
Share on other sites
MetalMarvels Newbie

MetalMarvels

Posted
  • Author
Posted

Don't know about others, but I put "TA,1" in the "psof" section as follows:

 

 

psof #Start of file for non-zero tool number

pcuttype

toolchng = one

if ntools = one,

[

#skip single tool outputs, stagetool must be on

stagetool = m_one

!next_tool

]

 

#add communications prep code

"TA,1", e

"%", e

n, *progno, "(", sprogname, ")", e

"(DATE=DD-MM-YY - ", date, " TIME=HH:MM - ", time, ")", e

pbld, n, *smetric, e

pbld, n, *sgcode, *sgplane, "G40", "G49", "G70", "G80", *sgabsinc, "H0", "E0", "Z0",e

 

 

cheers.gif

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
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...