Haas Toolroom Lathe

[CNCJerry]

Hmm, I see you have a M09 twice in your program cycles M09 is coolant off M08 is coolant on.

M08 (on)
G00 Z0.2
G82 X0. Z-0.3 P0. R0.2 F0.003
G80
G00 Z0.2
M09 (off)

 

[Duc]

I've used this to check gcode/NC code in the past. Give it a whirl.

NC Viewer // GCode Viewer and Machine Simulator

Powerful online GCode Viewer to simulate GCode files. NC Viewer is the best free gcode editor for verifying CNC and 3D printer files.

ncviewer.com

I'll this a shot.

We have a Okuma lahe that does not like to switch tools unless you have a T0000 at the end of each cycle.

(CENTER DRILL)
T2123
G54 G99
G97 S700 M03
G00 X0.
G00 Z0.2
M09
G00 Z0.2
G82 X0. Z-0.3 P0. R0.2 F0.003
G80
G00 Z0.2
M09
G00 X0. (SAFE TC POSITION)
G00 Z5. (SAFE TC POSITION)
T0000 (CLEARS TOOL AND OFFSET)
M01 (OPTIONAL STOP, I ALWAYS ADD THIS FOR OPERERTOR EASE OF SET UP)
(END OF CYCLE)

Changing to gang tooling setup stop the prompt for the tool change but also elimated the ask for the tool post but I can add the M01 optional stop and stop the spindle to unlock door.

Add a M30 at the end of your program. Resets the machine back to the begning of the program.

Will do.

Hmm, I see you have a M09 twice in your program cycles M09 is coolant off M08 is coolant on.

M08 (on)
G00 Z0.2
G82 X0. Z-0.3 P0. R0.2 F0.003
G80
G00 Z0.2
M09 (off)

Originally they were M09 but I change to M08 so I could run dry with the door open for testing purposes. Best mod was the door override switches.

 

[bdkw1]

Add a M30 at the end of your program. Resets the machine back to the begning of the program.

This ^^^^^ also make sure your setting to reset the defaults at M30 is on. Setting 56 I believe.

 

[bdkw1]

You also have a bunch of redundant lines and codes in there. Once G00 is called, you don't need to type it agian till you have call a code that cancels it like G1 or G81.

Also, G00 cancels drill cycles so no need to type G80. Your drill cycles automatically return to the R level, no need to give it a command to rapid to the R level since it's all ready there.

 

[Duc]

You also have a bunch of redundant lines and codes in there. Once G00 is called, you don't need to type it agian till you have call a code that cancels it like G1 or G81.

Also, G00 cancels drill cycles so no need to type G80. Your drill cycles automatically return to the R level, no need to give it a command to rapid to the R level since it's all ready there.

Tomorrow I will need to work thru all the code to remove alot of the extra along with adjusting the z retract distances. Probably wont add anything to the project but it will be a good education in lathe coding.

This ^^^^^ also make sure your setting to reset the defaults at M30 is on. Setting 56 I believe.

Changed in the settings.



First Test went really well. Feeds and speeds are slow for the prototype run but the fucker worked.



I have a few more parts on order to make the setup work better.
1. 4-port Loc-line manifold with nozzles to reduce the need to adjust coolant nozzle
2. Additional Tool blocks
3. Additional mounting block from tormach
4. Additional shims for the tooling blocks.


Few items I still need to figure out
1. Mounting the Dorian cut knurler on the right hand side using the additional Tormach block
2. a lathe tool for grooving and parting in one tool so everything stays mounted and there is no tool change till a completed part is done.

 

[CNCJerry]

Sweet looks like you have a good start.

We don’t have a HAAS in our shop but I have a post processor for HAAS TL, I was just curious what the code looks like out of Mastercam, you can clean up your code some but this comes with experience. I did notice the processer puts a T2100 at the end this is essentially the same as the T0000 I suggested earlier.

If you need help on more complex code let me know, I can knock out lathe programs pretty quick.

%
O1000(TEST PART)
(1/12/2023)
G00 G54 G18 G40 G80 G97 G99 G20
(TOOL - 21 OFFSET - 22)
(DRILL)
T2122
G97 S750 M03
G0 G54 X0. Z.25 M8
G83 Z-1. R.1 Q.1 P.1 F.0015
M9
G28 U0. W0. M05
T2100
M30
%

 

[bgaidan]

2. a lathe tool for grooving and parting in one tool so everything stays mounted and there is no tool change till a completed part is done.

If you haven't tried a GT grooving/parting insert yet, I'd recommend them. They're the only ones that consistently work perfectly in my little manual lathe. Every other one I've tried - from solid HSS, brazed and DGM style.

I use this shars "retrofit" one in a regular parting tool holder

But I really need to pick up one in this style for more rigidity when I don't need the length.

And I just learned that make GTR and L inserts for left and right parting - so you can actually fully part off and not leave a giant bur. All I've used are GTN. I need to find some GTRs.

 

[bdkw1]

You guys and your safety blocks

This isn't a Fanuc 6A. That shit resets itself.

 

[Duc]

You guys and your safety blocks

This isn't a Fanuc 6A. That shit resets itself.

Safety Blocks?


Any experience with the Kennametal Beyond Evolution groove/part off tooling? Looking into purchasing a tool holder with a size 3 insert to turn the profile and part the piece off.

 

[bdkw1]

Safety Blocks?


Any experience with the Kennametal Beyond Evolution groove/part off tooling? Looking into purchasing a tool holder with a size 3 insert to turn the profile and part the piece off.

This shit at the start of the program.

G00 G54 G18 G40 G80 G97 G99 G20

Unless your doing something funny, it's always gonna be G54. No cutter comp left or right on a lathe so no G40 needed.

Kennametal makes good stuff. We use a lot of their tools at work.

 

[gozuki]

This shit at the start of the program.

G00 G54 G18 G40 G80 G97 G99 G20

Unless your doing something funny, it's always gonna be G54. No cutter comp left or right on a lathe so no G40 needed.

Kennametal makes good stuff. We use a lot of their tools at work.

It's all default "cover your ass stuff" in virtually every post processor ever. Doesn't hurt anything except memory.

 

[bdkw1]

It's all default "cover your ass stuff" in virtually every post processor ever. Doesn't hurt anything except memory.

If you're still running an unmodified post processor, your leaving a lot on the table. Just because the default is crap doesn't mean you need to stick with it. My MC post will make programs that look almost like hand written ones.

 

[gozuki]

No doubt a modified post is the way to go as far as efficiency goes. No matter what I post, I end up going through it myself.

 

[Duc]

Getting closer to finishing off the project. Working on it here and there.

Had to install extra coolant nozzles to avoid moving it with each tool.

Not sure the modification to the Hardinge tool holder can be seen in the picture but I welded a 1/2in thick steel plate to the bottom of the tool holder before machining the tool holder to fit a 1 inch tool shank. Otherwise the bottom of the tool holder was a little thin. Programming the cut knurl is a little different than other tools. Im thinking its a issue with how Im setting the location or not sure what.

I touch off on the diameter of the rod before hitting the X Diameter measurement. Diameter measured 1.45inches

Data from the Dorian knurl excel spreadsheet. For testing I set DOC to .020 instead of the calculated .028

Program part for knurl
(Knurling)
T2124
G54 G99
G97 S316M03
M08
G00 X1.47 (Pushes the tool .020 into part, versus the normal setting it to 1.43)
G00 Z.2
G01 Z-.950F0.005
G00 X1.45
G00 Z1.5
M09
G00 Z4.0

Figure some of this is due to the machine setup since normally the tool is facing the other way.

 

[AlxJ64]

Are you getting any deflection out of the stock sticking out that far and if so is it compensated for in the feed numbers? This is a standard type knurler and not a cutting type, right? If so, knurling even on a manual lathe, seems to take a good bit of force. Dunno, just spitballing here from a manual machinist point of view. My CNC experience is 2D on a plasma table only and one college class where it was talked about for a day or two 20 years ago now.

 

[Duc]

Are you getting any deflection out of the stock sticking out that far and if so is it compensated for in the feed numbers? This is a standard type knurler and not a cutting type, right? If so, knurling even on a manual lathe, seems to take a good bit of force. Dunno, just spitballing here from a manual machinist point of view. My CNC experience is 2D on a plasma table only and one college class where it was talked about for a day or two 20 years ago now.

Very little or no deflection since it is a cut knurler. Found a new one on ebay for cheap

 

[bdkw1]

Interesting, I haven't seen a knurling tool like that. The diamond ones normally have angled grooves on the wheels.

 

[Duc]

Interesting, I haven't seen a knurling tool like that. The diamond ones normally have angled grooves on the wheels.

Ran into them when doing research into knurling on practical machinist. Much lower cutting forces, increased life on wheels and avoids pressing flake material back into the parent material. Issue that sometimes pops up during post treatment of parts.

Dorian catalog talks about it

https://www.doriantool.com/wp-content/uploads/2022/05/SEC-H-Knurling-Tools_LowRes_compressed.pdf

And you can haul ass if you want.

 

[bgaidan]

Interesting, I haven't seen a knurling tool like that. The diamond ones normally have angled grooves on the wheels.

Same. I had to look them up.

I use a scissor type on my little manual to take as much pressure off the cross and compound as possible, but those obviously aren't an option on a CNC.

 

[Duc]

Same. I had to look them up.

I use a scissor type on my little manual to take as much pressure off the cross and compound as possible, but those obviously aren't an option on a CNC.

You would be surprised. Normally I dont watch Titan but this did pop up during research.


And the video that conviced me to buy the cut knurling.

 

[bdkw1]

Ran into them when doing research into knurling on practical machinist. Much lower cutting forces, increased life on wheels and avoids pressing flake material back into the parent material. Issue that sometimes pops up during post treatment of parts.

Dorian catalog talks about it

https://www.doriantool.com/wp-content/uploads/2022/05/SEC-H-Knurling-Tools_LowRes_compressed.pdf

And you can haul ass if you want.

If your material is flaking while knurling something is wrong. To much pressure or not enough feed. But cutting looks like it would give a better finish on light knurls that have plateaus.

 

[bdkw1]

Also, the cutting one makes me think of skiving.

 

[gozuki]

Unrelated to anything, but Dorian makes some bad ass shit. For a smaller tool company, I'm impressed.

 

[Duc]

Finished off the lathe programming and start to run parts.

Might need to turn audio down. Filming from the top would be better but I dont care to get soaked by coolant. Each part takes around 3mins and 30 seconds. I will countersink the back side in the mill probably.



Not the sexist program but gets the job done

O01000(FACING CYCLE)
(SAFETY LINE BELOW)
G00 G54 G18 G40 G80 G97 G99
T1
G54
Z10.0
G50 S1800 (Max Spindle Speed)
G97 S720 M03
G00 X1.530
G00 Z0.2
M08
G96 S500 (Constant surface speed)
G71 P781 Q782 D0.040 U0. W0.001 F0.005
N781 G00 X1.375
G01 X.1 Z0.0
G01 X1.3000 Z0.0
G01 X1.3750 Z-0.090
N782 G01 X1.375 Z-1.25
G00 Z0.2
G97 S720
M09
G00 X1.5 (SAFE TC POSITION)
G00 Z1. (SAFE TC POSITION)



(CENTER DRILL)
T2121
G54 G99
G97 S750 M03
G00 X0.
G00 Z0.2
M08
G00 Z0.2
G82 X0. Z-0.3 P0. R0.2 F0.004
G80
G00 Z0.2
M09
G00 X0. (SAFE TC POSITION)
G00 Z2.5 (SAFE TC POSITION)

(END OF CYCLE)

(DRILL)
T2122
G54 G99
G97 S1000 M03
G00 X0.
G00 Z0.05
M08
G00 Z0.05
G83 X0. Z-1.1 R0.075 Q0.3 F0.003
G80
G00 Z0.05
M09
G00 X0. (SAFE TC POSITION)
G00 Z1. (SAFE TC POSITION)

(END OF CYCLE)

(TAP)
T2123
G54 G99
G97 S400
G00 X0.
G00 Z0.2
M08
G00 Z0.2
G84 X0. Z-0.95 R0.2 F0.0625
G80
G00 Z0.2
M09
G00 X0. (SAFE TC POSITION)
G00 Z1.5 (SAFE TC POSITION)
(END OF CYCLE)

(Knurling)
T2124
G54 G99
G97 S324 M03
M08
G00 X1.405
G00 Z.2
G01 Z-0.9 F0.006
G01 X1.365 F0.005
G00 Z1.5
M09
G00 Z4.0
M05
M00 (Verify part off tool is in)
(Part Off)
T404
G54
G50 S1800
G97 S600 M03
G00 X1.65
G00 Z0.1
M37 (PARTS CATCHER)
G00 X1.65
M08
G96 S400
G00 Z-0.88
G75 I0.725 X0.3 F0.002
G00 X1.65
G00 Z4.0
G97 S600
M09
G00 G53 X0.
G00 Z10.0 (SAFE TC POSITION)
M37 (PARTS CATHER DOWN)
M05
( END OD PART OFF CYCLE )

M00
(Change to Turning tool)

M30

 

[AKnate]

Where my brother works, they used to run mostly HAAS mills.
For a while it allegedly was the most HAAS equipment under 1 roof in the US.
Building is large enough they have bikes and electric golf cart truck things to get around.

Several years ago they scrapped them all and got high end Mori Sekei, Fadal, etc. Each setup was something like 3-4x what the HAAS units cost.

But speed and accuracy greatly improved. The $$ they saved from much less scrapping of parts, tooling, fixtures, and HAAS quickly paid for the equipment.

He said it was like going from a Walmart tool kit to Snap On.

I was surprised given the allegedly good name HAAS has.

 

[bgaidan]

high end ....Fadal

Wut?

 

[SomeGuyFromOlympia]

Where my brother works, they used to run mostly HAAS mills.
For a while it allegedly was the most HAAS equipment under 1 roof in the US.
Building is large enough they have bikes and electric golf cart truck things to get around.

Several years ago they scrapped them all and got high end Mori Sekei, Fadal, etc. Each setup was something like 3-4x what the HAAS units cost.

But speed and accuracy greatly improved. The $$ they saved from much less scrapping of parts, tooling, fixtures, and HAAS quickly paid for the equipment.

He said it was like going from a Walmart tool kit to Snap On.

I was surprised given the allegedly good name HAAS has.

Boeing?

 

[gozuki]

I worked at Haas for a few years. The most Haas equipment under one roof is in Oxnard.

 

[AKnate]

I worked at Haas for a few years. The most Haas equipment under one roof is in Oxnard.

Could be. They had that stuff for probably 15+ years, so maybe was back in the day, no idea.

 

[PAToyota]

Getting closer to finishing off the project. Working on it here and there.

Had to install extra coolant nozzles to avoid moving it with each tool.

Hmmm...

Looks somewhat familiar...

Several years ago they scrapped them all and got high end Mori Sekei, Fadal, etc. Each setup was something like 3-4x what the HAAS units cost.

Hopefully they found new homes and didn't actually get scrapped. Yes, the high end is much better, but a lot of little guys would love to have other's cast offs.