New to G-Coding

[Larry Myers]

Hi All,

I recently bought a Sharp 2412 VMC with a Fanuc Oi controller. I am totally new to writing G-code. My knee mill has a 3-axis Proto Trac M3 with canned cycles so that is what I am accustomed to.

I’ve written my first program and was really hoping that someone might be willing to look over it for me.

This is an aluminum disk, 8” od and .75” thick. It has a tapped center hole that is a 3/8-16 along with a .175” deep counter bore. Along the X axis are two holes at +3.5” and -3.5” that are 5/16-18. Then there is a 5/8” wide slot that is .45” deep along the Y axis.

You’ll see that I jump in tool numbers from T3 to T5. I deleted the block (?) that had tool #4.

Any criticism would be very helpful Thanks so much in advance.

PS: I sure hope a posting like this is OK. If not, please accept my apologies.

Larry

%
O0100(ADAPT PLATE)
T1M6(#4 CENTER DRILL)
G0G90G54X3.5Y0S4000M3
M8
G43H1Z.1
G81G98Z-.3R.1F20.
X-3.5
G80
G0Z.1M5
G81G98Z-.3R.1F20.
X0
G80
GOZ.1 M5
M9
G28G91Z0
M1

T2M6(#F DRILL)
G0G90G54X3.5Y0S3800M3
M8
G43H2Z.1
G83G98Z-1.1Q.08R.1F25.
X-3.5
G80
G0Z.1M5
M9
G28G91Z0
M1

T3M6(5/16-18 CUT TAP)
G0G90G54X3.5Y0
M8
G43H3Z1.
M29S350
G84G95Z-1.R1.F.0555
X-3.5
G80Z1.5M5
M9
G28G91Z0
M1


T5M6(.625 EM)
M8
G0G90G54X0Y2.99S5000M3
G43H5Z.1
G1Z-.1 F20.
Y1.89
G1Z-.2
Y2.99
G1Z-.3
Y1.89
G1Z-.4
Y2.99
G1Z-.45
Y1.89
G1Z.1F50.
M9
G28G91Z0

T6M6(5/16" DRILL)
G0G90G54X05Y0S3800M3
M8
G43H6Z.1
G83G98Z-1.25Q.09R.1F25.
X0
G80
G0Z.1M5
M9
G28G91Z0
M1


T7M6(3/8-16 TAP)
G0G90G54X0Y0
M8
G43H7Z1.
M29S350
G84G95Z-1.R1.F.0625
X0
G80Z1.5M5
M9
G28G91Z0
M1

T8M6(1/2" end mill)
G0G90G54X05Y0S2500M3
M8
G43H8Z.1
G81G98Z-.175R.1F10.
X0
G80
G0Z.1M5
M9
G28G91Z0
M1

M30
%
In the above (T8M6 sequence) G43 line, Z is 0.1". Then in the G81 line R is 0.1" I am trying to figure out the difference between the Z and the R. I think R is rapid (distance from the top of the part) If so, then what is the Z for? Thanks

[timlkallam]

Hello Larry I have Sharp mini mill also . You only use the R
if you want the drill or tap to retract to a different Z height from your start point. I like the tap or drill cycle to stop where i started it.If I start drill a Z.1 i want it to finish the cycle at Z.1 So I have no use for the R. Your machine boots up in the g98 mode so when you start a caned cycle like drilling or tapping the tool will retract to the same z height you started. So forget about the R.

This is how i would write the program .I like to keep the machine in G94 mode inchs per min. I notice you tap in G95 fed per rev. Either one will do the job but don't for get to change back to g94 after tapping.

Also no need to put in the G91 g28 z0 between tool changes when you call for a tool change the tool will go straight up to home anyway.


O0100(ADAPT PLATE)
T1M6(#4 CENTER DRILL)
G0G90G98G54X3.5Y0S4000M3
M8
G43H1Z.1
G81Z-.3F20.
X0
X-3.5
G80
M9
T2M6(#F DRILL)
G0G90G54X3.5Y0S3800M3
M8
G43H2Z.1
G83Z-1.1Q.08F25.
X-3.5
G80
M9
T3M6(5/16-18 CUT TAP)
G0G90G54X3.5Y0
M8
G43H3Z1.
M29S350
G84Z-1.F19.4444
X-3.5
G80
M9
T5M6(.625 EM)
M8
G0G90G54X0Y2.99S5000M3
G43H5Z.1
G1Z-.1 F20.
Y1.89
G1Z-.2
Y2.99
G1Z-.3
Y1.89
G1Z-.4
Y2.99
G1Z-.45
Y1.89
G1Z.1F50.
M9
T6M6(5/16" DRILL)
G0G90G54X05Y0S3800M3
M8
G43H6Z.1
G83Z-1.25Q.09F25.
X0
G80
M9
T7M6(3/8-16 TAP)
G0G90G54X0Y0
M8
G43H7Z1.
M29S350
G84Z-1.F21.875
X0
G80
M9
T8M6(1/2" end mill)
G0G90G54X05Y0S2500M3
M8
G43H8Z.1
G81Z-.175F10.
X0
G80
M9
G28G91Z0
Y0
M30

[Larry Myers]

Hi Tim,
Thank you so much. Your advise has been a huge help. This being my first time, I have been very apprehensive about what I am doing.

I have gone through what you wrote comparing it line by line to what I wrote. As such a few questions came to mind:

1)You said you like to keep the machine in G94 mode (inches p/min) Should I assume that is a default? I couldn’t find where you put G94 into your program.

2)If I did want to use G95 for tapping, would I place the G94 on the same line as the G80?

3)I saw you entered a G98 near the top line. You said it boots up to G98 as well. Is it just a precaution of some sort to put the G98 in as you did?

Again my sincere thanks. I sure do appreciate the help. This is such a cool place!

Larry

[timlkallam]

Hello Larry ,Glad to help

1)You said you like to keep the machine in G94 mode (inches p/min) Should I assume that is a default? I couldn’t find where you put G94 into your program.

Yes G94 is a defalt if you go to mdi mode you will see a list of g codes that a curently active or model when your machine boots up ( G0 G90 G94 G40 G20 G80 G54 G69 G17 G22 G49 G98 G67 G64 G15)

2)If I did want to use G95 for tapping, would I place the G95 on the same line as the G80?

The manual has it before the M29 on a line by itself.

3)I saw you entered a G98 near the top line. You said it boots up to G98 as well. Is it just a precaution of some sort to put the G98 in as you did?

I just did it to be safe in case you had it in G99 mode.You don't have to put it in.

Tim

[Larry Myers]

Thanks again, Tim. It sure does help.

I am going to try the program today and see what kind of mess I can make. I'll let you know how it goes.

Best regards,
Larry

Update: The program ran perfectly! My old machine took 42 min, to do the part. The new machine took less than 4 min. WOW! Thanks again!