Haas mill smoothness/corner round settings

[Pilot Plant Supervisor]

I'm going to cut a die in our Haas EC-1600. I noticed the control has settings for smoothness and corner rounding. What does everyone use for mold/die work? Do you use the G187 or just change the settings page?

[Mic6]

Whenever I highspeed rough or helical bore, I use G187 P1 to rough, then in my finishing toolpath I change it to G187 P3. I put it in the post because some times I forget to change the setting and the roughing gets all jerky. The "Rough" parameter loosens it up, but be sure to leave a little more stock than 2d contour or else your finished part will have marks.

[Pilot Plant Supervisor]

How much stock do you leave? I am running it now, but I only left .010" on walls and floors. Feedrates are 50 to 60 IPM. I hope I'm not gouging it!

[Mic6]

Normally 2d contour I leave .01, but with HSM and the Rough parameter I leave .02, but I'm feeding over 100ipm. What material are you milling?

[Pilot Plant Supervisor]

H13 tool steel. See the topic "Extrusion Die suggestion" in the Industrial forum for more on what I'm doing. (I'm not smart enough to link it)

[workmantm]

Whenever I highspeed rough or helical bore, I use G187 P1 to rough, then in my finishing toolpath I change it to G187 P3. I put it in the post because some times I forget to change the setting and the roughing gets all jerky. The "Rough" parameter loosens it up, but be sure to leave a little more stock than 2d contour or else your finished part will have marks.

 

My machines say to use "E" for the override, how old are yours? I've been fighting this problem on my VF1(1997) and VF4(1999) for surfacing and high feed on a radial paths just taking a nose dive in productivity. My manuals also reference Parameter 134 as being tied to the G187 command. I can't find any information on how changing that parameter will effect productivity. I may just have to call HFO Anaheim and see if they can give me some feedback. Parameter 134 is different from the factory on each machine. No clue if the VF4 was ever changed since I lost all that data when the Mainboard crashed on me about 15 months ago.

[Trevor Bailey]

i have those settings built into my post. just modified the mpmaster.

[Mic6]

Same Here!

 

[workmantm]

Let me Clarify, I'm one of Gcode's contract customers. I don't have the post options for the code. Does the G187 code actually post with a "P" command in there? I'm trying to modify older proven code to cut the cycle times on roughing. I've got a video of a part running that should have high feed passes, reality is it's not coming close because the control is not setup for it. I've been trying to tune the controls and code for better performance, but it's all pretty much a shot in the dark. Hoping that someone that is using this on the control can help give me guidance for how to reduce the cycle times there. Still trying to interface with G for optimizing our planning/execution, bu I don't always have a day to put the parts on hold.

[Trevor Bailey]

here is an example:

 

%

O0000 (OP-1)

(TIME - 11:45)

(T3 - 1/2 BALL ENDMILL )

(WCS NAME - TOP)

G00 G17 G40 G80 G90

T3 M06 ( 1/2 BALL ENDMILL)

G187 P1 E.02 - P1 is the rouging mode(1-rough, 2-medium, 3-finish) / E is the tolerance to be used in that mode

G00 G17 G90 G54 X-.0972 Y-6.4541 S8000 M03

G43 H3 Z1. M08

Z.1

G94 G01 Z-.5 F50.

~~~

G03 X2.4051 Y-3.6204 I-.1 J0.

G01 X2.3788 Y-3.5618

G00 Z1. M09

G187 - G187 by itself resets machine to normal operating parameters

M05

G91 G28 Z0.

G0 G90 G128 X0 Y0

M30

%

 

G187 can be on any block, but I always put it right after the tool call.

 

The P (smoothness), controls axis accel/deccel settings. It has 3 choices, 1 (rough), 2 (medium) and 3 (finish) when used with G187.

 

Using G187 P1 E0.050 will net you a faster cycle time, but the toolpath will can be inaccurate. Using a big tolerance like this will mean you will need to leave more stock for finishing. You will have to play with the settings to see what is tolerable for the path you have selected and how much material you want to finish with.

 

If i am 3d roughing, i will generally use G187 P1 E.02 - aluminum @ 8000 rpm, 300 ipm, opti-roughing path, 25% stepover using a 1/2 ball/bull end mill, leaving .02 for finishing.

[workmantm]

here is an example:

 

%

O0000 (OP-1)

(TIME - 11:45)

(T3 - 1/2 BALL ENDMILL )

(WCS NAME - TOP)

G00 G17 G40 G80 G90

T3 M06 ( 1/2 BALL ENDMILL)

G187 P1 E.02 - P1 is the rouging mode(1-rough, 2-medium, 3-finish) / E is the tolerance to be used in that mode

G00 G17 G90 G54 X-.0972 Y-6.4541 S8000 M03

G43 H3 Z1. M08

Z.1

G94 G01 Z-.5 F50.

~~~

G03 X2.4051 Y-3.6204 I-.1 J0.

G01 X2.3788 Y-3.5618

G00 Z1. M09

G187 - G187 by itself resets machine to normal operating parameters

M05

G91 G28 Z0.

G0 G90 G128 X0 Y0

M30

%

 

G187 can be on any block, but I always put it right after the tool call.

 

The P (smoothness), controls axis accel/deccel settings. It has 3 choices, 1 (rough), 2 (medium) and 3 (finish) when used with G187.

 

Using G187 P1 E0.050 will net you a faster cycle time, but the toolpath will can be inaccurate. Using a big tolerance like this will mean you will need to leave more stock for finishing. You will have to play with the settings to see what is tolerable for the path you have selected and how much material you want to finish with.

 

If i am 3d roughing, i will generally use G187 P1 E.02 - aluminum @ 8000 rpm, 300 ipm, opti-roughing path, 25% stepover using a 1/2 ball/bull end mill, leaving .02 for finishing.

 

Thanks, I've been using the G187 with only an E0.XXX call out. We keep the machines really tight to ensure we have accurate finished parts. I've never seen anything about the "P" variable and wonder if that applies on machines with the old controls like mine. V9.xx and V10.35. I'll be trying it out here in the near future as I have a couple of the parts getting ready to hit the shop floor in the next couple of weeks and I'll let you know if these old beasts can handle it.

[Trevor Bailey]

the old ones will take it. look for setting 85 on the control. the one right under it should be the default tolerance. the 85 setting controls the 1, 2 or 3 setting for smoothness.

[workmantm]

the old ones will take it. look for setting 85 on the control. the one right under it should be the default tolerance. the 85 setting controls the 1, 2 or 3 setting for smoothness.

 

I checked my control this morning and this is what I see on both of my old machines. Nothing below setting 85. Could setting 44 be part of my problem? I'll have to see if I have one of the videos I've shot of it running that show how much slower the machine gets on my radial moves while roughing. The only thing is that I am not using CC during roughing 90% of the time. I've loosened up Setting 85 as wide as E.250 just to see if I can see any reduction in cycle time without getting any net result. The "P" will be added on the next run that I have available to see if I get any net change to the cycle times.