Programming

[chakaloso]

How can I make the working part goes to the front of the operator after the program is done?

After the program is done M30 the machined part goes all the way to the bottom left.
I want the part to go in front of the operator

Thank You!

[axis]

sounds like you have programed a g28 into the end. move the part to where you want it at the end of the program then write the numbers down and put that at the end of the program before the m30.

[Geof]

Move the table to the position you want it to stop after a program and make a note of the machine coordinates. End your program with G53 G00 Xxxxx Yyyyy M30 where the xxxx and yyyy are the machine coordinates you noted.

[gar]

070306-2115 EST USA

chakaloso:

To add to Geof's comments.

Your machine home position is when the table is fully to the left, and fully to the front. This is where HAAS positions the table on startup, and is machine absolute zero. At this point the spindle is above the top rear corner of the table. If you press the POSIT key the absolute machine position is displayed under MACH, and will read 0, 0, 0 for X, Y, Z. This Z position is also the tool change position.

On our VF-2 if you hand jog to machine absolute -15.0000 the table will be in its mid-position, and fully to the front so Y still equals 0.

Consult your HAAS manual on G53. Note: it says this is a non-modal command which means it only applies to the one line it is on. Also it implies that X and Y values entered on the G53 line put the machine at that X, Y value relative to the machine absolute zero or home position.

Effectively G53 is a command to move the table to a position defined by the X and Y values specified relative to the machine absolute zero position. No G00 is required. So G53 X-20. Y-4. will move the table, no matter where it starts from, to the location X=-20., Y=-4. relative to machine home.

If the table started at home it would move 20" to the right and 4" to the rear. Or relative to the right rear corner of the table the spindle would move to x=-20" and y=-4" . Speed of motion is rapid. Thus, G53 is equivalent to G00 in speed.

.

[PBMW]

I use G53's all the time.
On my Minimill, I just remove the X 0.0 from the last G28 line. it only goes to Y zero after it lifts teh tool to Z zero.
I do it in the post processor.

[chakaloso]

HI

G53 works great.



I did exactly what you told me to do
before M30 I added G53 x-8.0 and I got the working piece in front of the door.

Thank You for your help.

[gar]

070307-0951 EST USA

Continuing the discussion:

As I previously mentioned G53 is a motion command. It does not set any variable locations that define a reference point, or offset. Rather it is a G00 motion relative to machine absolute zero. If I were writing the G-code interpreter I would use something like G0A instead of G53 for the command name. This would closely associate the command with G00 which it is identical to except for the reference point and being non-modal.

Whereas, G52, G92, a thing called COMM on the lathe, G54-G59, G110 etc. when combined in some fashion are offsets from machine absolute zero to determine the spindle position relative to the part. The execution of one of these commands selects or modifies something, but does not initiate a motion. Note: also that G10 falls in the category of modifying something.

People get hung up on the use of the terms "work shift" and "work offset", I see no real difference. There are a number of different variables that are added together to determine the spindle position relative to the part.

In the thread
http://www.cnczone.com/cg...3;t=004149;p=0
Seymour incorrectly associates G53 as a component summed with G52, G5x, etc. G53 does not belong in this sequence. However, Seymour did give a good presentation if G53 is left out. This summing of the various offset componernts to determine spindle position is something I discussed somewhere else.

The HAAS manual description relative to the relationship of G52, G92, and the G5xs and other components is very inadequate.

How does COMM differ from G92. The infromation is inconsistent in the on-line mill manual.

In lathe operations COMM presents the same problem as G52 on the mill in HAAS mode relative to being not reset except when explicitly zeroed. This is for the information of those that do not like G52 in HAAS mode on the mill.


For reference from the HAAS on-line manuals:

On the HAAS Lathe

#5201-#5206 Common offset
#5221-#5226 G54 work offsets
#5241-#5246 G55 work offsets
#5261-#5266 G56 work offsets
#5281-#5286 G57 work offsets
#5301-#5306 G58 work offsets
#5321-#5326 G59 work offsets

#7001-#7006 (#14001-#14006) G110 (G154 P1) additional work offsets
#7021-#7026 (#14021-#14026) G111 (G154 P2) additional work offsets
.....
#7361-#7366 (#14361-#14366) G128 (G154 P19) additional work offsets
#7381-#7386 (#14381-#14386) G129 (G154 P20) additional work offsets

#14401-#14406 G154 P21 additional work offsets
#14421-#14426 G154 P22 additional work offsets
.....
#15781-#15786 G154 P90 additional work offsets

15881-15886 G154 P95 additional work offsets
15901-15906 G154 P96 additional work offsets
15921-15926 G154 P97 additional work offsets
15941-15946 G154 P98 additional work offsets
15961-15966 G154 P99 additional work offsets


On HAAS Mill

On page describing offsets
#5201-#5205 G52 X, Y, Z, A, B OFFSET VALUES


Under MACROS

#5201-#5205 Common offset
#5221-#5225 G54 work offsets
#5241-#5245 G55 work offsets
#5261-#5265 G56 work offsets
#5281-#5285 G57 work offsets
#5301-#5305 G58 work offsets
#5321-#5325 G59 work offsets

#7001-#7006 (#14001-#14006) G110 (G154 P1) additional work offsets
#7021-#7026 (#14021-#14026) G111 (G154 P2) additional work offsets
.....
#7361-#7366 (#14361-#14366) G128 (G154 P19) additional work offsets
#7381-#7386 (#14381-#14386) G129 (G154 P20) additional work offsets

#14401-#14406 G154 P21 additional work offsets
#14421-#14426 G154 P22 additional work offsets
.....
#14561-#14566 G154 P29 additional work offsets
#14581-#14586 G154 P30 additional work offsets

etc like the lathe.

.

[Geof]

Originally Posted by chakaloso ...I added G53 x-8.0 and I got the working piece in front of the door...

-8.0 to move in front of the door; are you working with a MiniMill?

Here is another hint; put in G53 G00 Z3.5 and that will lift your tool up out of the way for unloading and reloading the vise.

[jackson]

I just use
G0 X (what ever direction you need to move)
G28 G91 Z0 Y0

[Geof]

Originally Posted by gar 070307-0951 EST USA Continuing the discussion: As I previously mentioned G53 is a motion command. It does not set any variable locations that define a reference point, or offset. Rather it is a G00 motion relative to machine absolute zero.....

According to the Haas manual G53 is a coordinate selection command:

"G53 Non-Modal Machine Coordinate Selection (Group 00)
This code temporarily cancels work coordinate offsets and uses the machine coordinate system. In the machine coordinate system, the zero point for each axis is the position where the machine goes when a Zero Return is
performed. G53 will revert to this system for the block it is commanded in."

When a move to a G53 coordinate is commanded it will use whichever motion command, G00 or G01, is active at the time. Or a motion command may be included.

It is correct that it does not set a variable reference point, it uses the fixed reference point of machine zero.

Jackson; Your; "G0 X (what ever direction you need to move)" will move to this X coordinate using whatever work coordinate (G54 to G??) is active at the time. If you want the table to stop at the same location relative to the door of the machine you need different X's for different work coordinate locations. It is much simpler to specify the location relative to machine zero using G53 because this is the same for any program.

[gar]

070307-1542 EST USA

Geof:

Last night on our 1993 VF-2 I checked G53 feed rate and it was rapid independent of any previous line containing G01. However, I did not check G01 on the same line as G53.

A command line
G53 X something
causes a motion but changes no accessable variables.

I think that the HAAS description is misleading to some extent.
Basically G53 is a motion command that uses machine absolute zero as its reference. If you issue G53 X something you get motion. If you issue G54 there is no machine motion, but you change the current coordinate system to G54.

In the HAAS description there is no mention of machine motion.


The equivalent function to G53 is to make a particular G5x, for example G59, all zeros. Then,

G54
....
G59
G00 X something or G01 X something
G54
....

is equivalent to G53 X something,

but this does not automatically revert to the previous G5x, I had to put in G54. However, I can write the code to avoid this problem if necessary, but it gets even more complex. That is the reason G53 exists.

.

[Geof]

Originally Posted by gar 070307-1542 EST USA Geof: Last night on our 1993 VF-2 I checked G53 feed rate and it was rapid independent of any previous line containing G01. However, I did not check G01 on the same line as G53....

I think Haas has changed things. Here are some motion commands in a small program. The G54 was at -70. in X and -45. in Y . The comments I added here.
%
O00000
N1 G00
N2 G28 Moves home
N3 G53 X-10. Rapid move
N4 G53 Y-10. Rapid move
N5 G54 Y20. Rapid move
N6 G54 X50. Rapid move
N7 G53 G01 X0. Y0. F400. Feed move
N8 G53 X-10. Feed move
N9 G53 Y-10. Feed move
N10 G54 Y20. Feed move
N11 G54 X50. Feed move
N12 G53 X-10. Feed move
N13 G53 Y-10. Feed move
N14 G54 Y20. Feed move
N15 G54 X50. Feed move
N16 M30
%

I ran this program through, then edited out the G00 on line N1and ran it again and all the motion was Feed.

If hit RESET and then ran the version without the G00 on line N1 the result was as below;

%
O00000
N1
N2 G28
N3 G53 X-10. Alarm No Feed Rate
N4 G53 Y-10.
etc

My conclusion is that the G53 motion does depend on the preceding G00 or G01. At the first run through the program ended with G01 active; this meant that when the line N1 G00 was removed the motion was still using the G01. When the feed was cancelled by RESET G01 was still active but with no feed rate. Adding a feed command at line N3 allowed it to run with all motion feed.

So I think the Haas manual as I copied it is correct with regards to the way the machines operate now. These tests were done on a 2005 Gantry Router.