[GUIDOSAN]

I have Mathews Precision 1330 running a Siemens 802s/c. It has been sitting since new while I try to understand the controller. I have it up and operating from MDA and Auto mode but it refuses to respond (or give an error code) to a g1 command. G0 and spindle commands work normal. Referencing is normal. It doesn't matter whether I am in mda or a program it just stops at a g1 command.

Help please.

[Al_The_Man]

Was an F (feed) command issued after the G01?
Al.

[GUIDOSAN]

yes - I set the default for inch and used f2 as a feedrate. The controller will issue an alert if the feed rate is not set on a g1 command. I used g1z-2f2

[Al_The_Man]

What does it show in the Distance-to-go readout if you have it?
Al.

[GUIDOSAN]

It shows the correct distance to go but it doesn't move.

[Machineit]

Did you put F2. or just F2? On most machines an F2 will be read like it is F.0002

[GUIDOSAN]

I tried both F2 and F1.5 but I will try again tonight to be sure my memory is correct. Just a great point though. I hope my memory is wrong.
I didn't think of that because on my Tormach (Mach3) the decimal is assumed unless placed.
I also called G95 even though the manual says its active unless G94 is called. (i tried G94 as well just to be sure but without results)

[GUIDOSAN]

Al,
I tried it again last night.
I used g1z-2f2.0
The distance to go showed 2 but no movement of the axis.
G0z-2 moves the axis and dro normally.

Guy

[Machineit]

You need to post your program.

Mike

[GUIDOSAN]

this is a test program I ran to check axis movement after referencing

G90 G70 G23 G94
M3 650
M0X-.50Z-1.5
M1Z-2.0F2.0
M2

all i was after was to start and set spindle speed, rapid move in 2 axis and a controlled move on the z axis.

I'm probably failing to do something very basic but I can't see it.
Guy

[Machineit]

this is a test program I ran to check axis movement after referencing

G90 G70 G23 G94
M3 650
M0X-.50Z-1.5
M1Z-2.0F2.0
M2

all i was after was to start and set spindle speed, rapid move in 2 axis and a controlled move on the z axis.

I'm probably failing to do something very basic but I can't see it.
Guy

I do not see an work offset in your first line, like G54 (this is your "work offset"), telling your control how far the part is from the X and Y home location. I also do not see a tool call-up like T1 and D01, (this tells the control how long your tool etc. the X and Z offset of the tool. Without these your lathe has no idea where anything is and will not move.

G94 is rate in inch/min, but you have not given a G96 or G97 to establish Constant Surface speed(changes rpm with diameter) or Direct RPM(same speed always) programming.

You are taking shortcuts with your code, spindle should be S650 not 650. Unless my Siemens controller is different than yours, G01 is G01 not M01 and G00 is G00 not M00.

G94, G95, is your feedrate either in inch/rev or inch/min. You must pair them with a spindle speed call G96 or G97.

I really think that you need to go back to the manual and study more. Look at some sample programs and see how the code it really written. Mine is old, but still has sample programs and an explanation of what each line of code does.

If you don't do this, you WILL crash. How much is costs you will be the question.

The following is a sub-program from my Siemens 810T control. It is using codes for a collet closer and a parts catcher, but you can get a general idea of a program. Remember this is a sub to a main program so the number will be different. Call your offsets, speeds and feeds, etc etc and try writing it correctly.

Mike

%SPF 1
G00 G40 G54 G64 F400 G70 G90 G95
H1020
G96 S1500 M03
G92 S1800
T1 ( C-DRILL )
G00 X0. Z.1 D1
G01 Z-.27 F.025
G00 Z.1
G00 Z8. D0
T2 ( #25 DRILL )
G00 X0. Z.1 D2
G01 Z-.58 F.025
G00 Z.1
G00 Z8. D0
T3 ( 10-24 TAP )
G00 X0. Z.1 D3
G97 S500 M03
G01 Z-.4 M03 S500 F.025
G01 Z.1 F.03 S500 M04
M05
G00 Z8. D0
T5 ( CUTTER FOR PROFILE )
G96 S1500 M03
G00 X.8 Z.1 D5 G96 M03 S1500
G01 Z0. F.005
G01 X.0
G00 X.715 Z.01
G01 Z0.
G01 X.75 Z-.03
G01 Z-.8
G00 X1.
G00 Z8. D0
T7 ( CUTOFF TOOL )
G00 X.9 Z.1 D7
G00 Z-.77
G00 X.755
G01 Z-.79 X.73 F.002
G01 X.1 F.008
G01 M26 X.15
G01 X-.05 F.008
G00 X1.0 M25
G00 Z6. D0
M05
T8 ( .75 BAR PULLER )
G00 X0. Z.1 D8
G00 Z-1.075
M21
G04 X2.0
G00 Z-.28
M22
G00 Z3.
M17

[GUIDOSAN]

Thank you Mike,

You're right - I was at work- I rushed through this from memory and shouldn't have. M1 obviouly doesn't translate to G1

Thanks for taking the time to respond and give an example. I'll study it and what I have for manuals. The controller did indicate the active tool was T4 and I did verify the parameters for the tool are correct so I didn't think I needed to call the tool. I'll try doing that tonight.

I'm slow in transitioning from my Tormach mill to this lathe but I'm determined to do it.

I appreciate your patience.

Guy

[Machineit]

Did you get it going yet?

Mike

[GUIDOSAN]

I took a break and finished a 12ga/45-70 side by side I was putting together. I'll dive back in when i get off work tomorrow. Thanks for asking.

[holbieone]

on some controls you need the spindle on to use G1

where G0 your just moving from one place to another

G1 you would be cutting

[GUIDOSAN]

Thanks for the idea - i'll check it out.

Mike,
On the program you posted I have a couple questions

n2 G00 G40 G54 G64 F400 G70 G90 G95

A) will the controller use the F400 feed rate as 4 inches/minute because of the implied decimal point - is it also correct to use 4.0 ?
B) why is there a G00 without a destination address?

what is H1020 ?

I have been reading Peter Smids programming handbook.

It's coming slowly into focus.
Guy

[holbieone]

Thanks for the idea - i'll check it out.

Mike,
On the program you posted I have a couple questions

n2 G00 G40 G54 G64 F400 G70 G90 G95

A) will the controller use the F400 feed rate as 4 inches/minute because of the implied decimal point - is it also correct to use 4.0 ?
B) why is there a G00 without a destination address?

what is H1020 ?

I have been reading Peter Smids programming handbook.

It's coming slowly into focus.
Guy

the G00 is modal and will stay so until another motion G code like G01 , G02 , G03 the G80's ext.


G00 ; CALLS RAPID MODE

X1.5 ; RAPID MODE

Y-2.5 ; RAPID MODE


G01F10.2 ; CALLS FEED MODE ,ON SOME CONTROLS A FEED RATE MUST BE SET HERE , SOME CONTROLS THE FEED RATE IS MODAL AND NOT NEEDED ON EVERY LINE

X.555 ; FEED MODE

Y3.114 ; FEED MODE

[Machineit]

Thanks for the idea - i'll check it out.

Mike,
On the program you posted I have a couple questions

n2 G00 G40 G54 G64 F400 G70 G90 G95

A) will the controller use the F400 feed rate as 4 inches/minute because of the implied decimal point - is it also correct to use 4.0 ?
B) why is there a G00 without a destination address?

what is H1020 ?

I have been reading Peter Smids programming handbook.

It's coming slowly into focus.
Guy

The F400 is part of the safe start line from the manual. It states that it sets the feed to 400 inches per minute. I believe that is for the maximum rapid rate, but not sure.

The H1020 is to set the delay for the collet closer. This insures that it is fully closed or open for each operation. This code equal a two second delay.

Mike

[GUIDOSAN]

Eureka - It's running!
Thanks very much to both of you for your patience and help.
I was doing several things wrong which you pointed out.

Merry Christmas and thanks for the help. Now I can keep chewing my way through this - carefully as Mike pointed out - single blocking my way along.
Guy