What's new
What's new

Hardinge VMC1000ii and Fusion 360 issues

cr250dave

Plastic
Joined
Jan 4, 2014
Location
Colorado Springs
Hi,

I am looking for some help with a new to me 2000 Hardinge and getting Fusion 360 CAM to work together. I am trying to do a simple part as shown below but I am running into problems with the CAM sending my machine into over-travel. I am not sure why it is telling the table to move in 2 inch moves during a 2D adaptive when the part is less than 2 inches wide. Depending on where the table is when I start the program determines how many lines in before it over-travels (roughly N105). It also never jogs over to where G54 is set before it travels off into nowhere. Oh and it has a Hardinge/Fanuc Control System II.

%
O1225 (SCDC TEST)
(T5 D=0.5 CR=0. - ZMIN=-0.75 - FLAT END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G20
N20 G28 G91 Z0.
N25 G90

(2D ADAPTIVE2)
N30 T5 M06
N35 S2140 M03
N40 G54
N45 M08
N55 G00 X-0.0491 Y-2.3205
N60 G43 Z0.6 H05
N65 G00 Z0.2
N70 Z-0.13
N75 G01 Z-0.18 F21.4
N80 X-0.049 Y-2.3202 Z-0.1856
N85 X-0.0487 Y-2.3193 Z-0.1911
N90 X-0.0484 Y-2.3178 Z-0.1965
N95 X-0.0478 Y-2.3157 Z-0.2017
N100 X-0.0472 Y-2.3131 Z-0.2066
N105 X-0.0463 Y-2.3099 Z-0.2112
N110 X-0.0454 Y-2.3063 Z-0.2154
N115 X-0.0444 Y-2.3023 Z-0.2191
N120 X-0.0432 Y-2.2978 Z-0.2223
N125 X-0.042 Y-2.2931 Z-0.225
N130 X-0.0407 Y-2.2881 Z-0.2272
N135 X-0.0394 Y-2.2829 Z-0.2287
N140 X-0.038 Y-2.2775 Z-0.2297
N145 X-0.0366 Y-2.2721 Z-0.23

2017-11-14_8-39-07.jpg
 
I suggest posting your question on the Autodesk Fusion CAM forum. They are usually very helpful, especially if you can share the whole project file. That way, folks can look upstream from the g-code, and figure out what is going on.


Sent from my iPhone using Tapatalk
 
Overtravel doesn't seem to be program related.
not sure what to make of the 2" dimension issue
what values are in your offsets?
 
I suggest posting your question on the Autodesk Fusion CAM forum. They are usually very helpful, especially if you can share the whole project file. That way, folks can look upstream from the g-code, and figure out what is going on.


Sent from my iPhone using Tapatalk

Thanks, will post it there.

doesn't seem to be program related.

what values are in your offsets?

For G54
Z= -18.982
X= 17.8602
Y= -7.3490

These are all based off of the machine zero.
 
what corner of table is spindle above when sent to home position?
top left?
 
Depends on where the table is when I start the program but I have had it over-travel in X and Y.

almost sounds like the machine is in incremental g91 mode

2" program "can't" overtravel a 20" machine. :scratchchin:
 
Your tool change macro might be poorly written - leaving your machine in G91 after a tool change. Add a G90 after the tool change. If that doesn't fix it - something is wrong with your machine.
 
Your tool change macro might be poorly written - leaving your machine in G91 after a tool change. Add a G90 after the tool change. If that doesn't fix it - something is wrong with your machine.

That is a very real possibility as the previous owner knew less than I do and that's not much. Let me pull the macro and have a look. It also isn't pulling tool 5...
 
That is a very real possibility as the previous owner knew less than I do and that's not much. Let me pull the macro and have a look. It also isn't pulling tool 5...

tool changer could be random, where tool in spindle doesn't match what the carousel reads.
just drop in a g90 after tool change, to see what happens. Really you should be able to see what mode you're in just be looking at the right display screen on CNC.
 
tool changer could be random, where tool in spindle doesn't match what the carousel reads.
just drop in a g90 after tool change, to see what happens. Really you should be able to see what mode you're in just be looking at the right display screen on CNC.

Here is the tool change

:9020(TOOL CHANGE SUB-PROGRAM)
IF[#1014GE1]GOTO10
IF[#1015EQ1]GOTO20
IF[#20EQ0]GOTO30
#1100=1
G91G30Z0M19
M76
#106=BIN[#1032]
IF[#106EQ#20]GOTO40
#101=#4001
#102=#4002
#103=#4003
#104=#4015
G17G91G80G00G63M75
G30Z0.M19
M72
M74
M17
G28Z0.
T#20
M17
G30Z0.
M73
M78
M71
G#101G#102G#103G#104
N40M77
#1100=0
M99
N10#3000=1(MAG. COUNTER D402 NE D407 )
M99
N20#3000=2(AFL/MLK/ZNG SIGNAL ON)
M99
N30#3000=3(TOOL CHANGE FORMATE ERR.)
M99
 
G17G91G80G00G63M75
G30Z0.M19
M72
M74
M17
G28Z0.
T#20
M17
G30Z0.
M73
M78
M71
G#101G#102G#103G#104
N40M77
#1100=0
M99
N10#3000=1(MAG. COUNTER D402 NE D407 )
M99
N20#3000=2(AFL/MLK/ZNG SIGNAL ON)
M99
N30#3000=3(TOOL CHANGE FORMATE ERR.)
M99

Joe was right, it seems
 
Added a G90 following the tool change and now I'm getting a 224 P/S Alarm on line N55.

N30 T5 M06
N35 S2140 M03
N40 G54
N45 M08
N55 G00 X-0.0491 Y-2.3205
 
G17G91G80G00G63M75
G30Z0.M19
M72
M74
M17
G28Z0.
T#20
M17
G30Z0.
M73
M78
M71
G#101G#102G#103G#104
N40M77
#1100=0
M99
N10#3000=1(MAG. COUNTER D402 NE D407 )
M99
N20#3000=2(AFL/MLK/ZNG SIGNAL ON)
M99
N30#3000=3(TOOL CHANGE FORMATE ERR.)
M99

Joe was right, it seems

Yeah looks like he nailed it. I took the tool change completely out and it seems to be working correctly now. What would you guys suggest I do to cleanly resolve the macro?
 
Added a G90 following the tool change and now I'm getting a 224 P/S Alarm on line N55.

N30 T5 M06
N35 S2140 M03
N40 G54
N45 M08
N55 G00 X-0.0491 Y-2.3205


Could be related to your ZERO position settings?
Is "Absolute" X-0.0491 Y-2.3205 within your travel reaches?


Is it safe to ass_u_me that this is a Fanuc?



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

Think Snow Eh!
Ox
 
Here is the tool change

:9020(TOOL CHANGE SUB-PROGRAM)
IF[#1014GE1]GOTO10
IF[#1015EQ1]GOTO20
IF[#20EQ0]GOTO30
#1100=1
G91G30Z0M19
M76
#106=BIN[#1032]
IF[#106EQ#20]GOTO40
#101=#4001 (STORE INTERPOLATION MODE)
#102=#4002 (STORE PLANE SELECTION)
#103=#4003 (STORE ABSOLUTE OR INCREMENTAL)
#104=#4015
G17G91G80G00G63M75
G30Z0.M19
M72
M74
M17
G28Z0.
T#20
M17
G30Z0.
M73
M78
M71
G#101G#102G#103G#104 (RESTORE PRIOR MODAL G CODES)
N40M77
#1100=0
M99
N10#3000=1(MAG. COUNTER D402 NE D407 )
M99
N20#3000=2(AFL/MLK/ZNG SIGNAL ON)
M99
N30#3000=3(TOOL CHANGE FORMATE ERR.)
M99

See the comments in the toolchange macro in red. The statements that store the current modal G codes should be placed just after the line #1100=1. The way it is now always stores 91 in #103 and always restores G91 when the restore line is executed.
 








 
Back
Top