I have a problem with the x axis on a fanuc lathe

So recently I started training for a cnc programer and I'm using fusion360 but the x axis will not go to where I tell it to. For example if fusion tells it to go to x5 it will always do it but when I measure the diameter it's 2mm or more bigger.BUT here's the interesting part. If i enter g1 x5 into the MDI it makes it how its supposed to. Also on the display it says its on x5(even tho its not) and the backplot looks right for more complicated parts.Also also we recently moved the lathe from one corner of the shop to the other so that may affect it somehow?
I'm still new to the cnc world so sorry if this is something simple but I will appreciate any suggestions and tips you have.

randomy220 said:

So recently I started training for a cnc programer and I'm using fusion360 but the x axis will not go to where I tell it to. For example if fusion tells it to go to x5 it will always do it but when I measure the diameter it's 2mm or more bigger.BUT here's the interesting part. If i enter g1 x5 into the MDI it makes it how its supposed to. Also on the display it says its on x5(even tho its not) and the backplot looks right for more complicated parts.Also also we recently moved the lathe from one corner of the shop to the other so that may affect it somehow?
I'm still new to the cnc world so sorry if this is something simple but I will appreciate any suggestions and tips you have.

Click to expand...

.
might be a tool comp issue.
.
dro calibration might need checking, zero return might need checking, work offset thats active might need checking
.
if tool is extra high or low that also will effect accuracy as diameter changes
.
obviously if lathe bed not level or twisted that will effect things too

Thanks for the quick reply but the bed was level and the tool was good(checked it twice). I wont be back at the shop until tuesday so i wont be able co check the first two but even if those are bad how do you explain it working how its supposed to when i enter the move command manually.

when you run a program or rather at end of last program and or when reset button is pressed the defaults are reset usually
tool comp is off
rapid or feed might be active depends
work offset is often G54 depends on parameters
on a mill default plane like G17,G18,G19 is set
.
anyway there is normally a screen to see what modal gcodes are active
.
many a part has been scrapped cause program uses G55 work offset and operator pressed reset and work offset went to default G54, just saying some programs will state a gcode like 2 or 10 pages or screens back. that can make restarts challenging

when you are in mdi you might not be entering all the modal commands needed. might not have correct work offset active. might not be using tool comp
.
when program running it might be stating commands that are causing problems. or missing gcodes that are needed

Im not sure what are the defaults but the program has both g54 and g18
%
1001
N10 G98 G18
N11 G21
N12 G50 S6000
N13 G28 U0.

(PROFILE1)
N14 T0101
N15 G54
N16 M8
N17 G99
.
.
.

Ok, so your absolute position on the screen says it's at X5, but the diameter it turned is 2mm larger?
Are you positive the tool is offset correctly?
Do you have a value in the TOOL WEAR page of 1MM? That value should be zero or close to it, usually.
Tell us how you set the tool initially.

I didn't bother with the wear settings nor with the tool radius because it was a new insert and the offsets were 0 (but now that I think about it I'm not sure because I usually don't change those settings)
Sorry for being so unsure about everything i recently got into cnc machining so I sometimes forget to change something and just leave them as default.

I think that you need to post your code.

2mm differential doesn't sound nearly enough to be a offset active / offset inactive situation.


---------------

Think Snow Eh!
Ox

Mtndew said:

Ok, so your absolute position on the screen says it's at X5, but the diameter it turned is 2mm larger?
Are you positive the tool is offset correctly?
Do you have a value in the TOOL WEAR page of 1MM? That value should be zero or close to it, usually.
Tell us how you set the tool initially.

Click to expand...

I’m with Mtndew on this. I bet there’s a value of +2mm left over in the X wear offset register for offset 01 that is showing up in the program but not when scootching around in MDI.

Randomy- hit the offset button to check the X “wear” (not “geometry”) offset value for offset 01. There will be an X value and a Z value. Zero that X value out if it isn’t already. Make any initial adjustments in the “geometry” offset during setup and only adjust the “wear” offset as the insert actually wears down. That way you can just reset your wear to 0 when changing inserts instead of trying to remember to reset your wear offset to, say, 2mm when putting in a new insert. Good luck!

I never use "WEAR", but why would MDI not account for WEAR + OFFSET both?
I'm not following the logic there... ???

-----------------

Think Snow Eh!
Ox

Ox said:

I never use "WEAR", but why would MDI not account for WEAR + OFFSET both?
I'm not following the logic there... ???

-----------------

Think Snow Eh!
Ox

Click to expand...

I guess it would only happen if he somehow got tool 1 in position without calling up the offset in MDI (i.e. “T01X5.” instead of “T0101X5.”).

It's a fanuc. T0101 is tool 1 offset 1. Will read both wear and geometry together.

I want to see the actual code too. I'm wondering if there's a TNRC call in there...

If the display says X5 and the part is at 7, it's most likely an offset that is just off.

Then again, maybe he's turning a 5mm dia. that's sticking out 2 inches, lol.

guest said:

It's a fanuc. T0101 is tool 1 offset 1. Will read both wear and geometry together.

Click to expand...

Hello jancollc,
T0101 will certainly call both Geometry and Wear Offsets, but there are a couple of alternative setting for Tool Call and Offsets. Via parameter setting, you can have the Higher Digits (left most digits)select:

1. Tool Number only with the Lower Digits selecting Geometry and Wear
2. Tool Number and Geometry with the Lower Digits selecting the Wear

Regards,

Bill

So the first 01 is the tool number and the other one is offset? I didnt know that and now that you put it that way it may be the source of the problem. Tool changing for me is pointless because the machine does not have any automatic tool changing.

randomy220 said:

So the first 01 is the tool number and the other one is offset? I didnt know that and now that you put it that way it may be the source of the problem. Tool changing for me is pointless because the machine does not have any automatic tool changing.

Click to expand...

Hello randomy220,
As others have suggested, Post a copy of your program, which will allow the Forum members to have a better understanding of your issue. The model of the Fanuc control will be a help also.

As stated in my previous Post, the component of the Tool Call Command that applies the Tool Offset is dependent on parameter setting. An example of your Tool Call Command will be a help.

Regards,

Bill

%
1001
n10 g98 g18
n11 g21
n12 g50 s6000

(profile1)
n14 t0101
n15 g54
n16 m8
n17 g98
n18 g97 s1430 m3
n19 g0 x44.534 z5.2
n20 g50 s5000
n21 g96 s200 m3
n22 g0 z1.614
n23 x27.093
n24 g1 x25.362 f80.
N25 x22.534 z0.2
n26 z-27.185
n27 g18 g3 z-29.562 i-4.028 k-1.188
n28 g1 z-35.524
n29 g3 x24.534 z-37.916 i-10.693 k-5.874
n30 g1 x27.362 z-36.502
n31 g0 z1.614
n32 x23.362
n33 g1 x20.534 z0.2 f80.
N34 z-25.63
n35 g3 x22.146 z-26.719 i-8.584 k-7.194
n36 x22.396 z-26.973 i-1.006 k-0.654
n37 x22.877 z-28.373 i-3.96 k-1.4
n38 g1 x25.705 z-26.959
n39 g0 z1.614
n40 x21.362
n41 g1 x18.534 z0.2 f80.
N42 z-24.582
n43 g3 x21.534 z-26.273 i-7.584 k-8.241
n44 g1 x24.362 z-24.858
n45 g0 z1.614
n46 x19.362
n47 g1 x16.534 z0.2 f80.
N48 z-15.119
n49 z-15.123
n50 z-16.623
n51 z-16.628
n52 z-23.763
n53 g3 x19.534 z-25.072 i-6.584 k-9.06
n54 g1 x22.362 z-23.658
n55 g0 z1.614
n56 x17.362
n57 g1 x14.534 z0.2 f80.
N58 z-13.859
n59 x15.31 z-14.078
n60 g3 x16.534 z-15.123 i-0.588 k-1.046
n61 g1 x19.362 z-13.709
n62 g0 z1.614
n63 x15.362
n64 g1 x12.534 z0.2 f80.
N65 z-3.364
n66 g3 x13.534 z-6. I-6.7 k-2.636
n67 g1 z-8.
N68 g3 x12.534 z-10.636 i-7.2
n69 g1 z-13.297
n70 x15.31 z-14.078
n71 x15.534 z-14.149
n72 x18.362 z-12.734
n73 g0 z1.614
n74 x13.362
n75 g1 x10.534 z0.2 f80.
N76 z-1.601
n77 g3 x13.534 z-5.987 i-5.7 k-4.399
n78 g1 x16.362 z-4.573
n79 g0 z1.614
n80 x11.362
n81 g1 x8.534 z0.2 f80.
N82 z-0.546
n83 g3 x11.534 z-2.339 i-4.7 k-5.454
n84 g1 x14.362 z-0.925
n85 g0 z1.614
n86 x10.323
n87 g1 x7.494 z0.2 f80.
N88 z-0.138
n89 g3 x9.534 z-1.02 i-4.18 k-5.862
n90 g1 x12.362 z0.394
n91 g0 z1.614
n92 x9.46
n93 g1 x9.283 f80.
N94 x6.455 z0.2
n95 g3 x8.494 z-0.529 i-3.661 k-6.2
n96 g1 x11.323 z0.885
n97 x11.334
n98 g0 x15.362
n99 z-1.666
n100 g1 z-9.222 f80.
N101 x12.534 z-10.636
n102 g3 x11.348 z-11.814 i-6.7 k2.636
n103 g1 z-12.963
n104 x13.534 z-13.578
n105 x16.362 z-12.164
n106 g0 z-11.228
n107 g1 z-10.399 f80.
N108 x14.176
n109 x11.348 z-11.814
n110 g3 x10.162 z-12.63 i-6.107 k3.814
n111 g1 x12.348 z-13.244
n112 x15.176 z-11.83
n113 x15.861
n114 g0 x19.362
n115 z-13.279
n116 g1 z-15.214 f80.
N117 x16.534 z-16.628
n118 g3 x15.31 z-17.669 i-1.2 k0.004
n119 g1 x14.534 z-17.888
n120 z-21.644
n121 x15.168 z-21.809
n122 g3 x16.459 z-22.873 i-0.554 k-1.064
n123 g1 z-23.737
n124 g3 x17.534 z-24.149 i-6.547 k-9.087
n125 g1 x20.362 z-22.735
n126 g0 z-17.357
n127 g1 z-16.945 f80.
N128 x18.061
n129 x14.534 z-17.888
n130 x12.534 z-18.45
n131 z-21.123
n132 x15.168 z-21.809
n133 x15.356 z-21.864
n134 x15.534 z-21.927
n135 x18.362 z-20.512
n136 g0 z-19.024
n137 g1 z-17.507 f80.
N138 x16.061
n139 x12.534 z-18.45
n140 x10.612 z-18.991
n141 z-20.623
n142 x13.534 z-21.384
n143 x16.362 z-19.969
n144 g0 z-19.668
n145 g1 z-18.048 f80.
N146 x14.14
n147 x10.612 z-18.991
n148 x8.69 z-19.531
n149 g2 x9.291 z-20.279 i2.722 k0.658
n150 g1 x11.612 z-20.884
n151 x14.44 z-19.469
n152 x17.069
n153 g0 x25.362
n154 z-25.526
n155 g1 z-28.147 f80.
N156 x22.534 z-29.562
n157 x22.396 z-29.773
n158 g3 x21.31 z-30.419 i-1.131 k0.4
n159 g1 x20.534 z-30.638
n160 z-33.911
n161 x22.352 z-35.363
n162 x22.409 z-35.411
n163 g3 x23.534 z-36.544 i-10.63 k-5.986
n164 g1 x26.362 z-35.129
n165 g0 z-30.138
n166 g1 z-29.695 f80.
N167 x24.061
n168 x20.534 z-30.638
n169 x19.018 z-31.064
n170 z-32.701
n171 x21.534 z-34.71
n172 x24.362 z-33.296
n173 g0 z-31.774
n174 g1 z-30.121 f80.
N175 x22.546
n176 x19.018 z-31.064
n177 x17.503 z-31.49
n178 x20.018 z-33.499
n179 x22.847 z-32.085
n180 g0 x26.879
n181 z1.592
n182 x5.484
n183 g1 x5.083 f80.
N184 x2.255 z0.177
n185 x4.859 z-0.501
n186 g3 x11.534 z-6. I-2.863 k-5.499
n187 g1 z-8.
N188 g3 x6.862 z-12.849 i-6.2
n189 g1 x14.33 z-14.949
n190 x14.414 z-14.981
n191 x14.479 z-15.022
n192 x14.52 z-15.071
n193 x14.534 z-15.123
n194 z-16.623
n195 x14.52 z-16.676
n196 x14.479 z-16.724
n197 x14.414 z-16.766
n198 x14.33 z-16.798
n199 x6.537 z-18.99
n200 g2 x7.894 z-21.043 i3.798 k0.116
n201 g1 x14.244 z-22.696
n202 x14.333 z-22.727
n203 x14.401 z-22.77
n204 x14.445 z-22.82
n205 x14.459 z-22.873
n206 z-24.264
n207 g3 x20.469 z-27.264 i-5.547 k-8.56
n208 g1 x20.511 z-27.307
n209 g3 z-29.44 i-3.017 k-1.067
n210 g1 x20.468 z-29.483
n211 x20.407 z-29.519
n212 x20.33 z-29.548
n213 x14.695 z-31.132
n214 x20.657 z-35.894
n215 x20.666 z-35.902
n216 g3 x23.533 z-40.993 i-9.759 k-5.496
n217 g1 x26.362 z-39.579
n218 x27.295
n219 g0 x44.534
n220 z5.2
n221 g97 s1430 m3

n222 m9
n224 m30
%

randomy220 said:

So the first 01 is the tool number and the other one is offset? I didnt know that and now that you put it that way it may be the source of the problem. Tool changing for me is pointless because the machine does not have any automatic tool changing.

Click to expand...

Yes. As Bill mentioned, the way the wear offset is treated is set by parameter.

T0100 normally will call up tool one with no offsets. If that parameter is set to incorporate the geometry offset with a T0100, then only the value in the wear offset will be ignored.

T0101 calls up tool one and applies both offsets, no matter how that parameter is set.

T0 cancels the offsets.

If you MDI: G0 T0101 X5.0 it should put the edge of the insert at X5.0.

Your program looks fine. You should make sure that the G54 X value is set to zero if your tool one geometry offset is measured from X home position.

THAT is an awfull lot of code to happen in an awfully small area!

I guess that's the diff between CAM code and Finger Code?


Well, no G41 or 42 in there.....


--------------------

Think Snow Ehj!
Ox

Ox said:

THAT is an awfull lot of code to happen in an awfully small area!

I guess that's the diff between CAM code and Finger Code?

Click to expand...

Yeah, 7 or 8 passes no canned cycles...