Rookie lathe question

[tubeguy]

Hello guys, I have V23 W/lathe and have a dumb question. Not being a lathe guy Im wondering. If you buy a lathe like a "swiss" were there isnt a turret and tool numbers but rather a tool plate. How do you call the tools / positions for each operation. Does BC allow for this or does it require hand codeing / fixing after the basic G code is made by BC?

Question #2. Any significant changes to lathe V 25? Ive heard both ways, no changes and minor changes, anyone have it and care to comment?

Similar Threads:

• basic question for rookie
• Rookie Question...3 axis vs 4 axis controller
• CNC Rookie Help!
• Rookie question: How to make a stepper motor run using only a battery ?

[aldepoalo]

tubeguy,

I think you are talking about gang tooling. I don't believe their would be any different programming other than a tool call, but I could be wrong. If there was like a special index move that didn't use a macro on the control then they could be scripted in.


The lathe software from V24 to V25 is the same. They did not make any improvements to the lathe tool path features. From V24 to V25 the changes that were made that effect the lathe are the drawing tools.

Stretch and preview changes the way you use the software for CAD, other than that no changes to the CAM for lathe.

[SeanDa]

We do not support swiss machining at this time.

[aldepoalo]

Sean,

I don't think he was asking if we support swiss, just the gang tooling.

But to make things clear, BobCAD CAM Lathe software is just 2 Axis at this time.

[tubeguy]

Maybe Im not even asking the question right. Yes Im talking about gang tooling as it would be on a kia lathe. The sort thats mounted on the cross slide. It would seem you could define each tool positon somehow and call it, right? But I also can see were there would be interference issues getting the tool away from the work. Again Im a rook on this and havent bought the machine for this reason. I need to understand what "it" needs better. If anyone has some insight on this please let us know what you think.
Thanks....

[SeanDa]

It does not support gang tooling also. This is not an item that can be scripted

[Machineit]

Not sure about this particular gang lathe, but most call out tool numbers just like a turret lathe.

I had one for many years and just touched off tool like a turret or a mill. Tool change position was just retracted all of the way in Z axis. Really very simple until you start setting it up for max speed and only retract just enough for each tool to clear. Most don't have much Z anyway.

Can't you do some tool change just calling tools and offsets? It has been years since I had the lathe but I am looking at one right now. Hate to think I could not use BobCAD, but what the hell,used to write just by hand anyway.


Mike

[aldepoalo]

I would think you could script the post "IF" something special was needed for the tool change. The best way to find out is to request a script and see what they say.

http://www.bobcad.com/wp-content/med...ng-request.pdf

[tubeguy]

I dont think I should have used the term "swiss" I guess theres more to that term then just a gang tool or tool plate type machine. My mistake. Were talking about a mostly typical machine but with a single moving plate that the tools are attached to. And a VFD driven head.

BTW were there any fixes from V23 to V24 in lathe for a few of the tool radius, comp and library issues?

[ranchak]

Sooo if BobCad doesn't do gang tooling that kind of sucks. When I bought my V25 I was told it didn't support live tooling, but I think I was told gang tooling was supported. I know I had mentioned that I was looking at an OmniTurn. I'm pretty sure that I was told that there was a PP available for it. I could be wrong... but I know I had asked about the lathe module. If BobCad doesn't support gang tooling what software are other guys using?

[SBC Cycle]

Sooo if BobCad doesn't do gang tooling that kind of sucks. When I bought my V25 I was told it didn't support live tooling, but I think I was told gang tooling was supported. I know I had mentioned that I was looking at an OmniTurn. I'm pretty sure that I was told that there was a PP available for it. I could be wrong... but I know I had asked about the lathe module. If BobCad doesn't support gang tooling what software are other guys using?

I would have to see a properly working program for a lathe with a gang tool setup but I see no reason this can't be done in BobCAD. I don't even see scripting as entirely necessary (depends on how much manual coding you want do). The controller should be doing all the work, BobCAD just needs to call the tool right and the user would need to be careful with the retracts between tool changes.

Might you have to lie a little bit? Of course.

[aldepoalo]

I spoke with Brad at Dynamic Machinery Resources and he is going to send me a sample posted program that runs the fagor 8055 on a gang tooling lathe.

This way we can see the code format, from there we will all know if BobCAD CAM can post the correct code or not. If there is something special needed in the code we will know what needs to be done with the post to make it work correctly.


http://www.youtube.com/watch?v=rj5UI2epDKI&feature=channel&list=UL]Dynamic Machine Resources GT27 CNC Lathe Turning.mov - YouTube

[tubeguy]

OK, thanks for looking into it, this is a great forum.....

[aldepoalo]

I did get a manual for the 8025TG Dynamic. At this time I am reviewing the information.


Here is a sample drawing:


free image hosting


Here is a sample program for the drawing:

%00110
N000 G90 G95 S3000 T1.1 M4 M8(TURNING TOOL)
N010 G00 X.77
N020 G00 Z0
N030 G01 X-.01 F.003
N040 G00 X.52 Z.01
N050 G01 Z-.634 F.006
N060 G00 X.55 Z.010
N070 G00 X.41
N080 G01 Z-.092
N090 G00 X.43 Z.01
N100 G00 X0
N110 G01 Z0 F.003
N120 G01 X.18
N130 G03 X.3 Z-.06 R.06
N140 G01 Z-.095
N150 G01 X.39
N160 G01 Z-.14 
N170 G01 X.5 Z-.3119
N180 G01 Z-.636
N190 G01 X.75
N200 G00 Z1.
N210 M01
N220 G90 G95 S1200 T2.2 M3 M8(.125 DRILL)
N230 G00 X0
N240 G00 Z.05
N250 G01 Z-.125 F.003
N260 G00 Z.1
N270 G00 Z-.115
N280 G01 Z-.250
N290 G00 Z.1
N300 G00 Z-.240
N310 G01 Z-.375
N320 G00 Z.1
N330 G00 Z1.
N340 M01
N350 G90 G95 S1000 T3.3 M3 M8(.05 WIDE GROOVE TOOL)
N360 G00 X.625
N370 G00 Z-.533
N380 G00 X.515
N390 G01 X.400 F.0015
N400 G00 X.515
N410 G00 X.75 Z1.0 M05 M09
N420 M30

Here is the coded commented out:

%00110
N000 G90 G95 S3000 T1.1 M4 Absolute IPR spindle 3000rpm Tool 1 direction counterclockwise
N010 G00 X.77 Rapid feed to X+.77 diameter
N020 G00 Z0 Rapid to face Z0
N030 G01 X-.01 F.003 Facing cut to X-.01 at .003 IPR
N040 G00 X.52 Z.01 Rapid to X+.52 Z+ .01
N050 G01 Z-.634 F.006 Feed to Z-.634 AT .006 IPR
N060 G00 X.55 Z.01 Rapid to X+.55 Z+.01
N070 G00 X.41 Rapid to X+.41
N080 G01 Z-.092 Feed to Z-.092
N090 G00 Z.01 Rapid to Z+.01
N100 G00 X0 Rapid to X0
N110 G01 Z0 F.003 Feed to Z0 AT .003 IPR, beginning of finish pass
N120 G01 X.180 Feed to X.18, start of radius
N130 G03 X.3 Z-.06 R.06 Generate a .06 radius
N140 G01 Z-.095 Feed to Z- .095
N150 G01 X.39 Feed to X+.39
N160 G01 Z-.14 Feed to Z-.14
N170 G01 X.500 Z- .3119 Feed along 10O taper
N180 G01 Z-.636 Feed to Z-.636
N190 G01 X.75 Feed off material to X+.75
N200 G00 Z1. Rapid to Z1., Safe position for next tool
N210 M01 Optional stop
N220 G90 G95 S1200 T2.2 M3 Start-up block for tool #2 .125 Drill 1200 rpm clockwise
N230 G0 X0 Rapid to X0
N240 Z.1 Rapid to Z.1
N250 G01 Z-.125 F.003 Feed to Z-.125 at .003 IPR
N260 G00 Z.1 Rapid out to Z+.1
N270 G00 Z-.115 Rapid into hole +.01 from last position
N280 G01 Z-.250 Feed to Z-.250 at .003 IPR
N290 G00 Z.1 Rapid out to Z+.1
N300 G00 Z-.240 Rapid into hole +.01 from last position
N310 G01 Z-.375 Feed to Z-.375 at .003 IPR
N320 G00 Z.1 Rapid out to Z+.1
N330 G00 Z1. Rapid to Z1., Safe position for next tool
N340 M01 Optional stop
N350 G90 G95 S1000 T3.3 M3 Start-up block for tool #3 Groove tool
N360 G00 X-. 625 Rapid to X-.625
N370 G00 Z-.533 Rapid to Z-.533, groove position
N380 G00 X-.515 Rapid to safe position above .5 turned diameter
N390 G01 X-.40 F.0015 Feed to X-.40 at .0015IPR
N400 G00 X-.515 Rapid out of groove to X-.515
N410 G00 X-.75 Z2.0 M05 M09 Rapid to safe Z position turn off spindle and coolant
N420 M30 End of program

The one issue tools cutting from the front side and back side of the part. Where BobCAD would only program from 1 side.... As far as the tool calls I do not see an index move for the tool position. Instead I see a tool number and offset.

Documentation:

T Tool number address

This a number between T1.1 and T32.32 that is used to specify the tool required.

The format for this number is T12.12 The 1st 2 digits are for the tool plate position of the tool.

This number indicates the location on the tool plate that the tool is at.
T12.12 The 2nd 2 digits are for the Geometry and wear offset to be applied to the tool selected.

In normal operation the 1st 2 digits are the same as the 2nd 2 digits T12.12

[aldepoalo]

Tool Offsets,

Ok with the control and setup the tool offsets are saved on the machine ( as expected) When you call a Tool number and offset there is not moment that happens. Un like a turret late that would advance the next tool to a cutting position, in this case there is no movement the machine makes when a tool is called.

So

If you have 3 Tools and you wanted them to go to X1 Z0


T1.1
G00 X 1
G00 Z0

This would bring tool 1 to X1 Z0

T2.2
G00 X1
G00 Z0

This would bring tool 2 to X1 Z0

T3.3
G00 X1
G00 Z0

This would bring tool 3 to X1 Z0

This is because the tool " zero point" is saved as a tool offset.

The program would need to be written so the machine would move in X first to advance to the tool station, then in Z...

Now where it getting a little strange is when you cut on the front or back side the the lathe.

BobCAD always program on just one side the the lathe. Where using Gang tooling you can cut in + X or - X.

I think in order to post code to support x+ and X - there would need to be a script written that will reverse the value of the X if and when needed.

This is what I have come up with so far. Any thoughts...

[moldmker]

[aldepoalo]

ok,

So what I've found is the negative X movement can be posted with out a script.

I have a simple file for everyone to look at and are interested in feed back.



hosting images

% ######,MX,
; (BEGIN PREDATOR NC HEADER)
; (MCH_FILE=LATHE.MCH)
; (LTOOL T1 M1 S3 O15. I.25 A60 C.0156 H0. D0. N1)
; (LTOOL T3 M3 S9 O0. I.125 A0 C.0156 H.5 D0. N3)
; (SCYL S3 X0 Y0 Z-4. D1.5 L4.)
; (HCYL S3 X0 Y0 Z-4. D0. L4.)
; (END PREDATOR NC HEADER)
N1 G90 G97 G95 F.015
N2 M9
N3 T1 D1
N4 G92
N5 M3
N6 G0 X1.3 Z.25
N7 G1 Z-3.2306
N8 G1 X1.3171 Z-3.2449
N9 G3 X1.32 Z-3.25 I-.009 K-.0053
N10 G1 Z-4.
N11 G0 Z.25
N12 G0 X1.1
N13 G1 Z-3.0639
N14 G1 X1.3 Z-3.2306
N15 G0 Z.25
N16 G0 X1.02
N17 G1 Z-2.9972
N18 G1 X1.1 Z-3.0639
N19 G0 X2.
N20 G0 Z1.
N21 M9
N22 T3 D3
N23 D3
N24 G92
N25 M3
N26 F.015
N27 G0 X-1.4077 Z-2.4209
N28 G1 X-.5713
N29 G0 X-1.4077
N30 G0 Z-2.5209
N31 G1 X-.5713
N32 G0 X-1.4077
N33 G0 Z-2.5544
N34 G1 X-.5713
N35 G0 X-2.
N36 G0 Z1.
N37M9
N38 M5
N39 M30

I can see the tool call and offset would need to be changed from

T3 D3 to T3.3




picture hosting

Using a 4 would normally be for ID cutting, but in this case we can use it for -X features.

So far I can't tell why the software wouldn't be able to post for gang tooling lathes..........

[aldepoalo]

1 G90 G97 G95 F.015
N2 M9
N3 T1 D1
N4 G92
N5 M3
N6 G0 X1.3 Z.25
N7 G1 Z-3.2306

Looking at this block, we would also have an issue as it's not a good idea to move both the X and Z at the same time to the art position. As it would be more likely to cause a crash.

The initial position should move in X first than Z, which should be a simple post tweak.

[aldepoalo]

Sample X + OD Rough

% ######,MX,
; (BEGIN PREDATOR NC HEADER)
; (MCH_FILE=LATHE.MCH)
; (LTOOL T1 M1 S1 O27.5 I.25 A35 C.0156 H0. D0. N1)
; (SCYL S3 X0 Y0 Z-7.0866 D2.9528 L7.0866)
; (HCYL S3 X0 Y0 Z-7.0866 D0. L7.0866)
; (END PREDATOR NC HEADER)
N1 G90 G97 G95 F5.
N2 M9
N3 T1 D1
N4 G92
N5 M3
N6 G0 X2.2327
N7 G0 X2.0528 Z.039
N8 G1 Z-4.6668
N9 G1 X2.2528
N10 G0 Z.039
N11 G0 X1.8528
N12 G1 Z-4.6668
N13 G1 X2.0528
N14 G0 Z.039
N15 G0 X1.6528
N16 G1 Z-4.6667
N17 G1 X1.6557 Z-4.6668
N18 G1 X1.8528
N19 G0 Z.039
N20 G0 X1.4528
N21 G1 Z-4.6428
N22 G1 X1.4635 Z-4.6458
N23 G1 X1.5138 Z-4.6552
N24 G2 X1.531 Z-4.6581 I.0238 K.058
N25 G1 X1.5868 Z-4.6641
N26 G2 X1.6063 Z-4.6651 I.0235 K.1914
N27 G1 X1.6528 Z-4.6667
N28 G0 Z.039
N29 G0 X1.2528
N30 G1 Z-4.5466
N31 G1 X1.2662 Z-4.5589
N32 G2 X1.2742 Z-4.5649 I.0238 K.0116
N33 G1 X1.3084 Z-4.5876
N34 G1 X1.353 Z-4.6099
N35 G1 X1.4058 Z-4.6299
N36 G1 X1.4202 Z-4.6339
N37 G1 X1.4528 Z-4.6428
N38 G0 Z.039
N39 G0 X1.0528
N40 G1 Z-1.2489
N41 G1 X1.0845 Z-1.2671
N42 G1 X1.1197 Z-1.2934
N43 G3 X1.1261 Z-1.2989 I-.0194 K-.0149
N44 G1 X1.1452 Z-1.3183
N45 G1 X1.1552 Z-1.3288
N46 G1 X1.1732 Z-1.3553
N47 G3 X1.178 Z-1.363 I-.0698 K-.0257
N48 G1 X1.1859 Z-1.3829
N49 G3 X1.1913 Z-1.3979 I-.4241 K-.0844
N50 G1 X1.1957 Z-1.4311
N51 G1 Z-4.4368
N52 G1 X1.1996 Z-4.4645
N53 G2 X1.2019 Z-4.4732 I.0389 K.0007
N54 G1 X1.2115 Z-4.4952
N55 G1 X1.2152 Z-4.5029
N56 G1 X1.235 Z-4.5294
N57 G2 X1.2401 Z-4.535 I.0249 K.0079
N58 G1 X1.2528 Z-4.5466
N59 G0 Z.039
N60 G0 X.8528
N61 G1 Z-1.18
N62 G3 X.8659 Z-1.1825 I-.017 K-.0543
N63 G1 X.9227 Z-1.1965
N64 G3 X.9404 Z-1.2022 I-.067 K-.1146
N65 G1 X.9793 Z-1.2152
N66 G3 X.9883 Z-1.2186 I-.013 K-.0218
N67 G1 X1.0344 Z-1.2388
N68 G3 X1.0422 Z-1.2428 I-.0225 K-.0257
N69 G1 X1.0528 Z-1.2489
N70 G0 Z.039
N71 G0 X.6528
N72 G1 Z-1.1611
N73 G1 X.6557
N74 G1 X.7039 Z-1.1627
N75 G3 X.7292 Z-1.1637 I-.0089 K-.1876
N76 G1 X.7791 Z-1.1687
N77 G3 X.8032 Z-1.1716 I-.0107 K-.07
N78 G1 X.8528 Z-1.18
N79 G0 Z.039
N80 G0 X.6051
N81 G1 Z-1.1611
N82 G1 X.6528
N83 G0 X6.
N84 G0 Z1.
N85M9
N86 M5
N87 M30

Sample X- OD Rough

% ######,MX,
; (BEGIN PREDATOR NC HEADER)
; (MCH_FILE=LATHE.MCH)
; (LTOOL T1 M1 S1 O27.5 I.25 A35 C.0156 H0. D0. N3)
; (SCYL S3 X0 Y0 Z-7.0866 D2.9528 L7.0866)
; (HCYL S3 X0 Y0 Z-7.0866 D0. L7.0866)
; (END PREDATOR NC HEADER)
N1 G90 G97 G95 F5.
N2 M9
N3 T1 D1
N4 G92
N5 M3
N6 G0 X-2.0611
N7 G0 Z.039
N8 G1 Z-4.6668
N9 G1 X-2.2211
N10 G1 X-2.2351 Z-4.6682
N11 G2 X-2.2415 Z-4.6701 I.005 K-.0126
N12 G1 X-2.2467 Z-4.6718
N13 G2 X-2.253 Z-4.6754 I.0052 K-.0078
N14 G1 X-2.2579 Z-4.6791
N15 G1 X-2.2611 Z-4.6868
N16 G1 Z-6.4782
N17 G0 Z.039
N18 G0 X-1.8611
N19 G1 Z-4.6668
N20 G1 X-2.0611
N21 G0 Z.039
N22 G0 X-1.6611
N23 G1 Z-4.6668
N24 G1 X-1.8611
N25 G0 Z.039
N26 G0 X-1.4611
N27 G1 Z-4.6451
N28 G1 X-1.4646 Z-4.6461
N29 G1 X-1.5066 Z-4.6539
N30 G3 X-1.5289 Z-4.6578 I-.0589 K.1488
N31 G1 X-1.5751 Z-4.6629
N32 G3 X-1.5978 Z-4.6648 I-.0157 K.0583
N33 G1 X-1.6557 Z-4.6668
N34 G1 X-1.6611
N35 G0 Z.039
N36 G0 X-1.2611
N37 G1 Z-4.5543
N38 G1 X-1.2652 Z-4.558
N39 G3 X-1.2742 Z-4.5649 I-.0322 K.0161
N40 G1 X-1.3083 Z-4.5876
N41 G1 X-1.355 Z-4.6109
N42 G1 X-1.4001 Z-4.6277
N43 G3 X-1.4195 Z-4.6337 I-.0326 K.0419
N44 G1 X-1.4611 Z-4.6451
N45 G0 Z.039
N46 G0 X-1.0611
N47 G1 Z-1.2537
N48 G1 X-1.0845 Z-1.2671
N49 G1 X-1.1197 Z-1.2934
N50 G2 X-1.1261 Z-1.2989 I.0194 K-.0149
N51 G1 X-1.1452 Z-1.3183
N52 G1 X-1.1552 Z-1.3288
N53 G1 X-1.1732 Z-1.3553
N54 G2 X-1.178 Z-1.363 I.0698 K-.0257
N55 G1 X-1.1859 Z-1.3829
N56 G2 X-1.1913 Z-1.3979 I.4241 K-.0844
N57 G1 X-1.1957 Z-1.4311
N58 G1 Z-4.4368
N59 G1 X-1.1996 Z-4.4645
N60 G3 X-1.2019 Z-4.4732 I-.0389 K.0007
N61 G1 X-1.2115 Z-4.4952
N62 G1 X-1.2152 Z-4.5029
N63 G1 X-1.235 Z-4.5294
N64 G3 X-1.2417 Z-4.5364 I-.0341 K.0119
N65 G1 X-1.2611 Z-4.5543
N66 G0 Z.039
N67 G0 X-.8611
N68 G1 Z-1.1815
N69 G1 X-.9159 Z-1.1949
N70 G2 X-.9323 Z-1.1995 I.0182 K-.0419
N71 G1 X-.9727 Z-1.213
N72 G1 X-.9865 Z-1.2178
N73 G1 X-1.0324 Z-1.2379
N74 G2 X-1.0419 Z-1.2427 I.0196 K-.0244
N75 G1 X-1.0611 Z-1.2537
N76 G0 Z.039
N77 G0 X-.6611
N78 G1 Z-1.1613
N79 G1 X-.7056 Z-1.1627
N80 G2 X-.7292 Z-1.1637 I.0077 K-.1648
N81 G1 X-.7791 Z-1.1687
N82 G2 X-.8032 Z-1.1716 I.0107 K-.07
N83 G1 X-.8611 Z-1.1815
N84 G0 Z.039
N85 G0 X-.6051
N86 G1 Z-1.1611
N87 G1 X-.6557
N88 G1 X-.6611 Z-1.1613
N89 G0 X-6.
N90 G0 Z1.
N91M9
N92 M5
N93 M30

[SBC Cycle]

Can you do both X- and X+ turning in the same setup with different tools? Looks like you got this under control here Al