Drill Retraction too high with G83 on Haas after Fusion 360 generated program

Toolsparky · Dec 10, 2020

Hi All. I am new to using the Haas Mini Mill 2 and Fusion 360
Has anyone had this problem or know how to resolve it?

I Created a drilling program using Fusion 360 CAM to try and centre drill 6 Holes 3mm deep from Z0 (Top of workpiece).
Within Fusion I think I have set my Heights correctly and from what I can see the NC code generated within the program looks OK and the graphic simulation looks OK.
When I run the program the Drill retracts up to around Z 14.mm before starting to feed down to Z0 and below at feed rate for the next 0.5mm incremental peck!
I think I am correct in saying that it shouldn't go higher than Z2. as per the previous line to the Canned cycle.

I cant see anything in the program that instructs it to do this and I have checked setting 52 to make sure that's OK. I have tried setting 52 at 0.00 and 0.1mm but the drill still retracts to Z14.

Am I missing a machine parameter that I need to adjust or something?

Generated program is below
%
O10005
(Using high feed G1 F5000. instead of G0.)
(T1 D=10. CR=0. TAPER=118deg - ZMIN=-3. - drill)
N10 G90 G94 G17
N15 G21
N20 G53 G0 Z0.

(09129)
N25 T1 M6
(Adjust speeds/ feeds to suit)
N30 S1200 M3
N35 G54
N40 M8
N45 G0 X-32.72 Y0.
N50 G43 Z4. H1
N55 G0 Z2.
N60 G98 G83 X-32.72 Y0. Z-3. R2. Q0.5 F50.
N65 X-21.12
N70 X-9.04
N75 X3.04
N80 X15.43
N85 X30.27
N90 G80
N95 G0 Z4.

N100 M5
N105 M9
N110 G53 G0 Z0.
N115 X0.
N120 G53 G0 Y0.
N125 M30

%

Delw · Dec 10, 2020

Toolsparky said:
Hi All. I am new to using the Haas Mini Mill 2 and Fusion 360
Has anyone had this problem or know how to resolve it?

I Created a drilling program using Fusion 360 CAM to try and centre drill 6 Holes 3mm deep from Z0 (Top of workpiece).
Within Fusion I think I have set my Heights correctly and from what I can see the NC code generated within the program looks OK and the graphic simulation looks OK.
When I run the program the Drill retracts up to around Z 14.mm before starting to feed down to Z0 and below at feed rate for the next 0.5mm incremental peck!
I think I am correct in saying that it shouldn't go higher than Z2. as per the previous line to the Canned cycle.

I cant see anything in the program that instructs it to do this and I have checked setting 52 to make sure that's OK. I have tried setting 52 at 0.00 and 0.1mm but the drill still retracts to Z14.

Am I missing a machine parameter that I need to adjust or something?

View attachment 307170

Generated program is below
%
O10005
(Using high feed G1 F5000. instead of G0.)
(T1 D=10. CR=0. TAPER=118deg - ZMIN=-3. - drill)
N10 G90 G94 G17
N15 G21
N20 G53 G0 Z0.

(09129)
N25 T1 M6
(Adjust speeds/ feeds to suit)
N30 S1200 M3
N35 G54
N40 M8
N45 G0 X-32.72 Y0.
N50 G43 Z4. H1
N55 G0 Z2.
N60 G98 G83 X-32.72 Y0. Z-3. R2. Q0.5 F50.
N65 X-21.12
N70 X-9.04
N75 X3.04
N80 X15.43
N85 X30.27
N90 G80
N95 G0 Z4.

N100 M5
N105 M9
N110 G53 G0 Z0.
N115 X0.
N120 G53 G0 Y0.
N125 M30

%

Thats some f'k up code

try this
O10005

T1M6
G00 G90 G54 X-32.72 Y0.
S1200 M3
G43 Z4. H1 M8
G0 Z2.
G98 G83 X-32.72 Y0. Z-3. R2. Q0.5 F50.
X-21.12
X-9.04
X3.04
X15.43
X30.27
G80 <<<< NOT NEEDED ON A HASS
G0 Z4. M09
G91 G28 Z0.0
G91 G28 X0.0 Y0.0
M30

NO CLUE WHY YOUR USING G53 AND THAT MANY TIMES. OR AT ALL

Toolsparky · Dec 11, 2020

Thanks for your help with this Delw.
I tried your code but the spindle still retracted to approx 14mm. I thought to myself that this must be a Machine parameter issue now so I scrolled through the settings and saw that Setting 22 was set at 12.7mm. In the description this is described as canned cycle retract but the instructions just mention G73.
Thought I would try it set at 1mm and now the retraction is fine.
Thanks again.

cj.abraham · Dec 11, 2020

Delw said:
NO CLUE WHY YOUR USING G53 AND THAT MANY TIMES. OR AT ALL

G53 is the Haas-recommended method of homing the machine in a program. It's called out multiple times because the X move switches back to the active work offset and finds the center of the part and centers it in the door to present to the operator. G91 G28 X0. sends the table to the side of the machine which is not convenient for loading.

13engines · Dec 11, 2020

I was thinking this was a parameter problem. On another note...

Delw said:
G0 Z4. M09
G91 G28 Z0.0
G91 G28 X0.0 Y0.0
M30

NO CLUE WHY YOUR USING G53 AND THAT MANY TIMES. OR AT ALL

I'm with you... no line numbers. Unless you typically collaborate in email or over the phone about programs, what are they good for other then memory eater-uppers. (We Faunuc folks have to concern ourselves with such things.) I think they also make the blocks harder to read, but that could just be me not being used to them being there... doing nothing. :-)

I'm also with the G53 crowd. Better and safer way to move the machine to where you want it.

Perhaps our man forgot, but the machine was left in Incremental mode. Not something I would recommend.

Delw · Dec 11, 2020

cj.abraham said:
G53 is the Haas-recommended method of homing the machine in a program. It's called out multiple times because the X move switches back to the active work offset and finds the center of the part and centers it in the door to present to the operator. G91 G28 X0. sends the table to the side of the machine which is not convenient for loading.

Well haas is wrong on using the g53

it can be dangerous.

to get the machine to have vises goto the door is stupid simple. I only put the "X" in there cause thats what he had. Only time I even sent the x to the switchs is during power up because I have to. otherwise my end lines always reads.
if there long parts and I need to goto center of table I simply run the x to the middle of the table and then the code below.
My cad will do the automatically or I can add it manually if needed.

G0 Z4. M09
G00 X8.0 <<< using 2 6 inch vices or where ever your middle is.
G91 G28 Z0.0
G91 G28 Y0.0
M30

G91 G28 Z0.0
G91 G28 Y0,0
M30
every single mill I have run in 30+ years I use the same ending code never had issues yet on the controls I have used.

coyoinu · Dec 11, 2020

ya i've had op's problem bite me before.

if the machine is acting weird like this, a good thing to do is go into settings and hit ORIGIN to reset any lingering values like this.

Search

Largest Manufacturing Technology Community on the Web

Search

Drill Retraction too high with G83 on Haas after Fusion 360 generated program

Toolsparky

Plastic

Delw

Stainless

Toolsparky

Plastic

cj.abraham

Plastic

13engines

Stainless

Delw

Stainless

coyoinu

Aluminum

Similar threads