Delta 20 Drill cycle not working

[athis]

Hello all,

I have a Tree Journeyman 325 with a Delta 20 controller.



The drill cycle stops at the line with the G83. (N10) and sits there.

N1(T)OP3-SEQ-DRILL250-TOOL7$
N2(E)M6T7$
N3(E)S1800M3$
N4(E)G01X-4.66Y-.875F50.0$
N5(E)Z5.25$
N6(E)G80$
N9(E)Z4.4$
N10(E)G83X-4.66Y-.875Z3.925R4.4K.125Q.0625F20.0$
N12(E)G80$
N13(E)Z5.25$
N14(E)M5$
N15(E)M30$
END$

I've tried dozens of editing combination's...including adding an "N11" which for some odd ball reason the post processor didn't put out.

I also input the data into the controller (MDI) under Type event E for EIA.
The machine will not drill past the same point as the program above.
Does anyone happen to know why? Can someone post a drill cycle example to compare with?

Your help is greatly appreciated. This is my first post, please excuse anything I may have missed in terms of info.

Thx,
Athis

[underthetire]

I used the conversational mode on that control the most, but I think you need a G0 on line 13. I'm not used to seeing the Z heights and depths in positive geometry, so it's kinda throwing me off tonight.

[athis]

I used the conversational mode on that control the most, but I think you need a G0 on line 13. I'm not used to seeing the Z heights and depths in positive geometry, so it's kinda throwing me off tonight.

I understand. The machine is being programmed with cam, and posted for the delta 20 controller. I inserted the G0 on line 13, but since it doesn't read past line 10, it offered no help. The positive geometry is simple due to the coordinate system on the part. Z 0 happens to be below the hole by 4.8 inches.

[rock4xfab]

Here is a sample of what I use on a small production part.

N1(T)xmem .1325 Drill$
N2(T)5x2x.375 Plate$
N3(9)M03 E01 T01 S1400$
N4(9)M07$
N5(0)X.5Y0Z-.5 F8 G1 W+.05$
N6(0)X3.75Y0$
N9(0)X-4.55Y.5$
N10(0)X4.55Y-.5$
N12(0)G0$
N13(0)X-1Y0Z+1.1$
N14(9)M9$
N15(9)M05$
N16(9)M00$ use as a part change
N17(6)X0Y0F3T020$ This is repeat cycle First line N003 Times to repeat 20
N18(9)M30$


My tool is touched off of the part and Z Axis set to 00000..So E01 in the fixture offset reads X0Y0Z0 and tool table is
Z0 D.3125

[athis]

Thanks Rock4xfab,

I will give that a try and see what happens. Worst case scenario, I can edit my post processor to output Z values.

[jagardner4]

It's possible that the Z axis isn't moving within the In-Position range at the end of it's move. In-Position is only checked after a rapid move. Since you have G01 (Linear Feed) programmed in N4, the first rapid move involving the Z axis is your G83 in N10 when the Z axis has to rapid to the reference plane.

Put the control into "TM4 - Servo Adj" by going to the Setup Mode (Mode 5) and pressing "T", "M", "4" and then the "Enter" key. Re-run your program, and when the control "hangs," check how much lag is present on the Z axis. If it's more than .0005", the Z axis drive needs to be balanced.

[athis]

Jagardner4,

I do in fact have a Z issue on my mill. My Tree will not rapid in Z because the "pots" need to be adjusted. I've know that from the time I've purchased the machine. Not knowing how to fix that issue just quite yet, I have resorted to make sure my rapid moves are feed rated. Anything over 200ipm looses my Z.
If the Z rapids I get a servo error.

According to what you stated, it sounds like this may be my issue. I never thought it would affect a feed rated drill program though.

[rock4xfab]

Jagardner4,

I do in fact have a Z issue on my mill. My Tree will not rapid in Z because the "pots" need to be adjusted. I've know that from the time I've purchased the machine. Not knowing how to fix that issue just quite yet, I have resorted to make sure my rapid moves are feed rated. Anything over 200ipm looses my Z.
If the Z rapids I get a servo error.

According to what you stated, it sounds like this may be my issue. I never thought it would affect a feed rated drill program though.

After thumbing through my book.... G83 is not recognized in the dynapath control... That is a normal Fanuc G code. Dump it..

Also looking back at your line it apears you are starting and stoping or righting a drill cycle for each hole. With Dyanpath you dont need to .. Just tell G1 on and then just position movements.. It will continue to drill untill you tell it to stop. with a G0

[jagardner4]

With the control in TM4, as described in my earlier post, and with the Jog mode screen displayed, check the Z axis lag while the axis is sitting still. It's suppose to be zero, but will typically be + or - 0.0002". If it is greater than 0.0005" in magnitude, that's why the Z axis "hangs" at the end of a Z axis rapid move.

If your axis servo drives are Servo Dynamics, the pot you want to adjust is on the board for the Z axis and is labelled "BAL" (for balance). Adjust this pot with the servos on (but sitting still) until you get as close to zero as you can. This should alleviate your immediate issue, but the drives probably need tuning.

[T0DD]

Greetings Athis,
The following works fine on Delta 20 on a J325:

(0001)
N1T1M06
N2S900M03
N3G00X1.1345Y.655
N4Z.1
N5G83X1.1345Y.655R.1K.05Z-.25F2.
N6X1.1345Y-.655
N7X0.0Y-1.31
N8X-1.1345Y-.655
N9X-1.1345Y.655
N10X0.0Y1.31
N11X.364Y.9854
N12G80
N13G00Z1.
N14M30
E
If your machine hangs up on z rapid, you could program a high feed rate and turn the feedrate override down. Let me know how it works!
Todd

[athis]

Thanks for your input guys. I will try some of these solutions as soon as I get a chance.