Hello all, i recently purchased a used Sharp SV-2412S and am in the process of getting it up and going. It has a Fanuc OI-MC control. I am having trouble with what i believe is the CAM program coming out of Fusion 360. I have a pretty simple program loaded and when I run the program the spindle just takes off from wherever it is "parked" towards the front of the table. It does not seem to reference the work offset position at all. If i jog the spindle to a different position and start the program, it just starts from that new "parked" spot. My absolute coordinates are reading correct based on the work offset, but the spindle location doesn't read anywhere remotely close to the x-y position of the program. My G54 00 (EXT) are all 0's like it should be.
If i go to MDI mode and insert a simple program like below and hit cycle start, the spindle moves to the G54 work offset 0 and 1 inch above the stock.
G54 ;
G43 H01 ;
G00 X0 Y0 Z1 ;
I've posted the beginning of my G-Code, is there anything glaring such as work offset cancel that would be causing this? I come from hobby level Mach III so a fanuc control is new to me.
With the spindle part way down and the table sitting in any random position, what happens when you MDI T1M6? (Making sure the machine doesn't already think T1 is in the spindle) That would be of help to know.
Can you see what the number of the active program is on the screen during a tool change? It may be 9001 like dcoupar said. If so, look in that program and see what's in it. If you don't see a 9000 series program in your directory you'll have to change a parameter to be able to see and/or modify it. Though on my i control I'm password protected out of some parameter changes. If you don't see any 9000 programs then the tool change is likely handled by the PMC, and there is little you can see or do about it.
I don't see anything at the beginning of your code that should cause unplanned movement. Though try eliminating the G91G28Z0 in line 20 and see what happens. G28 moves typically have an intermediate position they go to on their way home to 0. Even though Z only goes up and down, it's worth a shot.
FYI - you talk of the spindle movements that are essentially X Y position movements. For example I would juxtapose -spindle takes off towards the front of the table, to table takes off towards the rear of the machine. The spindle does not move laterally, the table does. The spindle only moves up and down. You're the first person I can think of that talks of this kind of stuff this way. I can get where you're coming from, but I'm thinking it's not the way a person should express themselves when talking machine movement. Maybe there are those that will strike me down on this. Guess we'll have to see.
A couple pointers on the code generated by your post. There's not a lot of extra garbage like you see sometimes, but I do see other things.
T1 M06 (BULL NOSE/ADAPTIVE 1)________-Start with tool change and tool/process name.
G17G20G40G49G54G80G90G94G98 ______-Why not all prep codes in one line?
G00 X-0.638 Y-0.7256 ___________________-Move to start position while Z axis is home safe. (which your post did)
G43 Z0.2 H01 S7000 M3 T3 ______________-Bring tool to clearance plain with length offset/Get spindle ramping up/Pre-stage carousel.
M08 _________________________________-Coolant on when head is down at work and not high up spraying coolant who knows where.
The rest is fine. 13 lines down to 5. Same machine actions. Same initial position. I'd also like to suggest eliminating line numbers. They're not at all needed, they take up memory, (Which with Fanuc can cost you dearly.) and clutter the screen. If you need line numbers here and there because of calls by subroutines and the like, just add as needed, but not every line as a staple. Some people put a line number in front of each tool change to search to, but you can down arrow search T5 just as easily as N5. If you're per-staging tools you have to do it twice, but we're still talking only a couple seconds of difference.
My apologies for getting a little side tracked, just trying to help, but still... let us know what you come up with on your tool change problem.
Dave
Last edited by the_gentlegiant; 12-01-2019 at 01:44 PM.
Reason: Edited positioning language line.
Reply with Quote
Sharp CNC not going to start position
