G68.2 & G54.4

[So not a Guru]

I'm trying to get our new post working & I need a better understanding of TWP (G68.2) & WSEC (G54.4).

Can both of these be used simultaneously? The post I have is outputting this:

 

N100
(DRILL THREE FLANGE HOLES)
M08
G0 G20 G40 G80 G90
T9 T11 M6 (.252 DRILL)
G90 G0 G53 Z0.
G53 X0. Y0.
G54 G17
B90.0607 C279.1419
G68.2 X0. Y0. Z0. I9.142 J90.061 K0.
G53.1 P1
G65 P9544 H1 (CALCULATE G54.4 DYNAMIC OFFSET)
G54.1 P300 (CENTER OF ROTATION WPC)
G54.4 P1
X6.3883 Y-.4663 S3486 M03 M51
G43 H9 Z7.4511
G94
G98 G81 Z3.3511 R3.7011 F13.94
G80
G69
G53.1
G54.4 P0
G53 Z0.

 

Is that correct?

 

Zeke

[crazy^millman]

I'm trying to get our new post working & I need a better understanding of TWP (G68.2) & WSEC (G54.4).

Can both of these be used simultaneously? The post I have is outputting this:

 

N100

(DRILL THREE FLANGE HOLES)

M08

G0 G20 G40 G80 G90

T9 T11 M6 (.252 DRILL)

G90 G0 G53 Z0.

G53 X0. Y0.

G54 G17

B90.0607 C279.1419

G68.2 X0. Y0. Z0. I9.142 J90.061 K0.

G53.1 P1

G65 P9544 H1 (CALCULATE G54.4 DYNAMIC OFFSET)

G54.1 P300 (CENTER OF ROTATION WPC)

G54.4 P1

X6.3883 Y-.4663 S3486 M03 M51

G43 H9 Z7.4511

G94

G98 G81 Z3.3511 R3.7011 F13.94

G80

G69

G53.1

G54.4 P0

G53 Z0.

 

Is that correct?

 

Zeke

 

What does the machine builder have for documentation? I have seen where somethings that people that the machine could do it could not because it was never purchased. Implementing new processes sometimes require some testing and just going through some different types of operations to dial it in.

[So not a Guru]

What does the machine builder have for documentation? I have seen where somethings that people that the machine could do it could not because it was never purchased. Implementing new processes sometimes require some testing and just going through some different types of operations to dial it in.

I'm not sure what the machine builder supports. I've called & emailed them, but as yet, haven't gotten any clear answers. We actually have two new posts, one is for a Mazak VCU 500 & the other is for a Mazak Variaxis i800. I'm trying to sort thru the manuals now.

[Watcher]

I'm not sure what the machine builder supports. I've called & emailed them, but as yet, haven't gotten any clear answers. We actually have two new posts, one is for a Mazak VCU 500 & the other is for a Mazak Variaxis i800. I'm trying to sort thru the manuals now.

The manuals will cover everything but it doesn´t mean you have all functions they list. You need to look at the machine datasheet to see which options were ordered with the machines. It should be somewhere within the electrical cabinet.

[crazy^millman]

I'm not sure what the machine builder supports. I've called & emailed them, but as yet, haven't gotten any clear answers. We actually have two new posts, one is for a Mazak VCU 500 & the other is for a Mazak Variaxis i800. I'm trying to sort thru the manuals now.

 

Is this a brand new install or is this the 1st time you have been able to dig into these machines?

[So not a Guru]

Is this a brand new install or is this the 1st time you have been able to dig into these machines?

Both, the Variaxis is still being installed right now, But the VCU has had a post that never worked right for 5 axis work, despite our reseller's best efforts at modifying it, so we decided to purchase a new post for it from Postability.

[So not a Guru]

Am I correct in assuming that G41/G42 can be used while G68.2 & G43 is active?

Also, can G41.2/G42.2 be used while G54.4 & G43.4 is active?

[jlw™]

is this a mazak?  depending on the situation i run G68, G68.2 and G54.4

[So not a Guru]

is this a mazak?  depending on the situation i run G68, G68.2 and G54.4

Yes, it is a Mazak.

Am I on the right track to assume G68.2, using G43, on all 2D, 3D & 3 + 2 toolpaths, and G54.4, using G43.4, on all 5 axis simultaneous toolpaths? As well as using G61.1 & G05 P2 for 5X paths?

What situation would need G68?

[jlw™]

you are correct.  I use plain old G68 in the integrex's so I can spin C with out having to retract.  If you use G68.2 you need to fire off the G53.1 inclined planes which is a motion causing command (it's what "activates" the deviation from center)  It is the same as WPC Shift in a mazatrol program.  This is bad when your close to the part.  With plain old G68 you can still use all your cycles but it does not account for deviation from center of rotation so I only use it on part that we indicate.  G68 will also work with G54.4 if you need to account for center of rotation.  All of my 5 ax is table/head or head/head so I don't have any trunion machines.

[crazy^millman]

Both, the Variaxis is still being installed right now, But the VCU has had a post that never worked right for 5 axis work, despite our reseller's best efforts at modifying it, so we decided to purchase a new post for it from Postability.

 

Sorry about the issues with the original post, but will say you are in good hands.

 

On the new machine I would lay all of this out and go over it all with the AE that will be doing the machine training. Get your examples and do what you can to test it while they are there. Getting them back in after because something was not setup right can drag things on.

 

JLW has done it that way I have done it on the Integrex Machines. Nice to see it in action and glad to see it being supported better in the newer controls. When everything is dialed in and working like it is supposed to life is really good.

[jlw™]

I use postability for all of mine.  If you know what to ask for they will hit it every time.  And i have thrown some curves with this versatech.

[So not a Guru]

you are correct.  I use plain old G68 in the integrex's so I can spin C with out having to retract.  If you use G68.2 you need to fire off the G53.1 inclined planes which is a motion causing command (it's what "activates" the deviation from center)  It is the same as WPC Shift in a mazatrol program.  This is bad when your close to the part.  With plain old G68 you can still use all your cycles but it does not account for deviation from center of rotation so I only use it on part that we indicate.  G68 will also work with G54.4 if you need to account for center of rotation.  All of my 5 ax is table/head or head/head so I don't have any trunion machines.

Thanks, I do have G53.1 active with the G68.2 as well.

[So not a Guru]

What about G41.2 & G42.2? Can I use them when G54.4 is active?

[crazy^millman]

Depends on the machine and where you need the builder to give you all the feedback about what is and is not supported.

[jlw™]

What about G41.2 & G42.2? Can I use them when G54.4 is active?

Are these all new machines you're just getting now? Any have smoothx?

[So not a Guru]

Are these all new machines you're just getting now? Any have smoothx?

The Variaxis has it.

[jlw™]

Ran it much yet?

[So not a Guru]

Ran it much yet?

They are still setting it up. I have not been able to work with it at all yet. I am hoping to have the post ready by the time they get it up, but I am having a hard time getting the info I need from Mazak.

[jlw™]

Wow, I'm shocked by that! I never have any trouble. What info do you need?

 

You can see your options by doing this:

 

(IF memory serves)

Left menu key,

Left menu key,

Diagnosis,

Version,

Options (I think)

 

I'll get my hands on a panel this morning and tell you where to look. Every Mazak I've had my hands on will tell what options he has installed.

 

You also need to do a little parameter poking to get g68.2 working properly. You also need to do some parameter poking if you want to use mazatrol tool data where you don't call H and D words.

[jlw™]

Who are the guys installing it? Not that I would know probably, we get service from south eastern tech center.

 

Every one of these guys can get you a copy of the acknowledgement sheet, it will list options too.

[So not a Guru]

Wow, I'm shocked by that! I never have any trouble. What info do you need?

 

You can see your options by doing this:

 

(IF memory serves)

Left menu key,

Left menu key,

Diagnosis,

Version,

Options (I think)

 

I'll get my hands on a panel this morning and tell you where to look. Every Mazak I've had my hands on will tell what options he has installed.

 

You also need to do a little parameter poking to get g68.2 working properly. You also need to do some parameter poking if you want to use mazatrol tool data where you don't call H and D words.

I know how to find the options, but the descriptions don't reference the associated "G" codes. For example; we have "5 axis tool comp", is that G41.2/G42.2? We have "High smoothing control", is that G61.1 or M821-M830?

I'm going to call Mazak again today, hopefully I'll have better luck this time.

[Colin Gilchrist]

I know how to find the options, but the descriptions don't reference the associated "G" codes. For example; we have "5 axis tool comp", is that G41.2/G42.2? We have "High smoothing control", is that G61.1 or M821-M830?

I'm going to call Mazak again today, hopefully I'll have better luck this time.

 

PM me your email address and I will send you a copy of the PDF files from Mazak that cover Tool Length Comp and 5 Axis Cutter Comp. Both PDF files do a great job of explaining each function, and what modes have a conflict. For some of your questions, the answer just boils down to personal preference. (Do I want "G43.4" or "G43.5"? --> The answer depends only on if you want to see rotary angles (B/C) in your code, or do you prefer Vector (I,J,K) output? The advantage with Vector output is that the code is much more easily "transferred" to a similar sized machine with different kinematics. If you were moving the job to a different Mill/Turn that had A/C instead of B/C, then you would most likely need to re-post the NC code.

[Colin Gilchrist]

2-2 Offset Data Items Used for Tool Radius Compensation

 

The data settings of the TOOL DATA display (prepared for the execution of MAZATROL

programs) can also be used in tool radius compensation for five-axis machining. The table below

indicates those usage patterns of the externally stored tool offset data items which are applied to

the tool radius compensation according to the settings of the relevant parameters (F92 bit 7 and

F94 bit 7).

 

 

Parameter Data in the TOOL DATA display Data in the TOOL

F92 bit 7 F94 bit 7 ACT-φ ACT-φ CO./No. OFFSET display

 

0 0 × × @

0 1 × @ ×

1 0 @ × @

1 1 @ @ ×

@: Used for tool radius compensation.

×: Not used.

2-1 Programming Format

 

1. Tool radius compensation for five-axis machining ON

 

G41.5 (X_ Y_ Z_ B_ C_ D_);

G42.5 (X_ Y_ Z_ B_ C_ D_);

 

G41.5 : Tool radius compensation (to the left) [group 07]

G42.5 : Tool radius compensation (to the right) [group 07]

XYZBC : Axis motion commands

D : Tool offset data No. for radius compensation

 

 

2. Tool radius compensation for five-axis machining OFF (cancellation)

 

G40 (X_ Y_ Z_ B_ C_);

G40 : Cancellation of tool radius compensation [group 07]

2-3 Operation of Tool Radius Compensation for Five-Axis Machining

 

2-3-1 Startup of the tool radius compensation

 

The G41.5 or G42.5 code given in the cancellation mode turns on the mode of tool radius

compensation for five-axis machining, and describes such an initial offset path to the G41.5 or

G42.5 block’s ending point as includes compensation in the plane perpendicular to the tool axis

in that position. The startup operation in the compensation plane is the same as for the general

mode of tool radius compensation.

Take care to give the startup code, G41.5 or G42.5, under the appropriate conditions of G-codes

(see the table concerned in Section 3-1); otherwise an alarm will be caused (962 CAN NOT USE

G41.5, G42.5).

 

 

2-3-2 Operation in the mode of tool radius compensation

 

In the mode of G41.5 or G42.5 the tool radius compensation for five-axis machining only applies

to commands of positioning (G00) and linear interpolation (G01). Take care not to use G-codes

unavailable in the mode (see the table concerned in Section 3-1); otherwise an alarm will be

caused (961 G41.5, G42.5 MODE IS ACTIVE).

 

As for motion blocks automatically interpolated for turning a corner, the direction of the tool axis

at the ending point of the first one of the two blocks concerned (as specified in the last B-axis

command) is kept intact, along with the rate of feed and other modal information items, up to the

stop point for the single-block operation.

 

 

2-3-3 Cancellation of the tool radius compensation

 

The mode of tool radius compensation for five-axis machining is cancelled when one of the

following conditions is satisfied:

1. The cancellation command concerned (G40) is executed,

2. Zero is specified as the number of offset data for radius compensation (D00), or

3. The NC is reset.

 

 

2-4 Method of Computing the Offset Vector

 

This section describes how the compensation with respect to the diameter of the tool is

performed three-dimensionally by taking account of axis motion commands for rotating the axis

of the tool and the workpiece on the table. Let us now take as an example the machining of the

side faces of the workpiece by simultaneously rotating the workpiece and the tool axis on the Cand

the B-axis.

[Colin Gilchrist]

3-2 Restrictions

 

- The calculated path of tool radius compensation cannot be checked for interference,

irrespective of the setting of the parameter concerned (F92 bit 5: Checking to avoid interference

ON/OFF).

 

- The radius compensation codes G38 (to set an offset vector) and G39 (to interpolate a circular

arc at a corner) are not available in the mode of G41.5 or G42.5.

 

- Corner chamfering or rounding commands are not available in the mode of G41.5 or G42.5.

 

- The tool change command, if required, must always be given after cancelling the mode of

G41.5 or G42.5.

 

- Manual interruption in general, MDI interruption, and interruption by the manual pulse handle in

particular, cannot be used in the mode of G41.5 or G42.5.

 

- Tool radius compensation for five-axis machining is not available if the C-axis control of the

turning spindle No. 2 is concerned (on accordingly executed machines).

 

- The function in question cannot be used at all in the mode of operation for turning.

 

- Take the following precautions for compound use with the tool tip point control:

 

 

1. The tool radius compensation for five-axis machining must be turned on and off within the

mode of tool tip point control.

 

<Programming example>

G43.4 H1 (Tool tip point control ON)

・・・

G41.5 D2 (Tool radius compensation ON)

・・・

・・・

G40 (Tool radius compensation OFF)

・・・

G49 (Tool tip point control OFF)

 

2. The tool tip point control must have the workpiece coordinate system selected (with F85

bit 2 = 1) for describing the tool path in the program. Otherwise (i.e. when the parameter

F85 bit 2 is set to 0 to use the table coordinate system in programming) an alarm will be

caused (962 CAN NOT USE G41.5, G42.5) by the selection of the mode of tool radius

compensation for five-axis machining even with the above condition being satisfied.