Tool change homing routine edit

[Anonymous]

Hi. I have recently acquired a CNC lathe which has been retrofitted with a chinese SZGH-CNC1000TDb-2 controller, it's apparently Fanuc based and proven programs off another machine with a proper Fanuc control have run through it exactly as they should.

To set the tool offsets it seems the control sets G53 X and Z to zero at the tool reference point for each tool, which means in order to use G53 to move my turret back to the machine home point I need to remember whatever the offset is for that particular tool and edit the program accordingly. I don't know if this is normal, it's my first time away from Mach3 and also with an ATC, but from searching the internet for what I can about this control (can find nothing about it) and proper Fanuc controls, it seems the real ones have a measure function and a proper tool offset/position table which this doesn't have. The tool menu only has tables for wear and nose radius compensations.

G281 and G283 both work ok but they are painfully slow to move off the switches and will add a lot on to the cycle time.

I have found a way to work around this by first calling out a non existant tool (T0000) and then using G53 to rapid the turret out of the way and back to the machines X0 Z0 point. How can I get fusion to make this the standard tool change routine? I made a quick file up and the Fanuc turning post to see what it does and by default it puts G28 at the end of the toolpath before each change, which my controller doesn't accept (it has to be individual - G281 and G283).

[dmartinS68QJ]

We use Fanuc controllers for both MILL and LATHE and G28 is used to return home.  We only use WCS and tool wear compensation on our mills only, not for Lathes.  So G53 is used only on our mills to cancel WCS.   On our MILLs with dual pallets we do not use the WCS table of controller but have our own macros to set appropriate locations.  This allows main program to call G54, but have each pallet a unique physical location so pallets don't have to match 100%.

It sounds like you already have an idea you want T00 G53 added for each tool change.  That should be a fairly easy modification to the post processor.    See this answer helps get you in the right area, seems very similar and should get you going in the right direction.

https://forums.autodesk.com/t5/fusion-360-computer-aided/m01-between-same-tool-numbers/m-p/7721346#M...

Dan

[Anonymous]

Thanks. Looking at that I can't make head nor tail of the code/language there and what to put where.

Also looking further in to the controller manual it looks like the controller doesn't have G84, and G74 is apparently a peck drilling cycle. It says to use G93 for tapping instead?

I have seen the OD threading cycle in action which works ok. Spindle and both axis motors are encoded.

I'll guess I'll have to find someone who knows what they're doing to edit a post for this control if I want it to be up and running parts quickly? Is this something autodesk can/will do or will I have to find some other professional?

I'm a paid subscriber if that makes any difference.

[Anonymous]

Here is a link to the manual

[Anonymous]

Sausage fingers! Is there not an edit post button?

Anyway, manual link

http://www.szghauto.com/uploads/2015/06/231743288820.pdf

[dmartinS68QJ]

I am not familiar with that controller so I'll point you toward additional links:

http://cam.autodesk.com/posts/

https://knowledge.autodesk.com/support/hsm/learn-explore/caas/sfdcarticles/sfdcarticles/Post-Process...

[Anonymous]

Ok I have managed to make the change to the homing routine in the post and change the canned cycles I have to the correct g codes for the control.

I don't have all the canned cycles that fusion wants to output, in particular drilling where the only drilling cycle I have is for peck drilling (G73). How can I change other types of drilling cycles in the post to output using normal G01 X/Z movements instead? I can't figure this one out for myself what so ever.

Thanks.

[dmartinS68QJ]

Nice work figuring out how to modify the post, I believe it will server you well.  As for modifying different drill cycles you will need to find this function

function onCyclePoint(x, y, z) { 

....

somewhere within onCyclePoint should be a case statement for the various drill options.   If you have only drill then you could comment out all others cases except drill & default.   Default would be for any option that does not match any other statement.   Or get rid of all the case statements and use only the drill option.

switch (cycleType) {
case "drilling":

writeBlock(
gRetractModal.format(98), gCycleModal.format(81),
GetCommonCycle(x, y, z, cycle.retract, cycle.clearance),
feedOutput.format(F)
);

break;    //   End of case: "drilling"

case "counter-boring":
if (P > 0) {
writeBlock(
gRetractModal.format(98), gCycleModal.format(82),
getCommonCycle(x, y, z, cycle.retract, cycle.clearance),
"P" + milliFormat.format(P),
feedOutput.format(F)
);
} else {
writeBlock(
gRetractModal.format(98), gCycleModal.format(81),
getCommonCycle(x, y, z, cycle.retract, cycle.clearance),
feedOutput.format(F)
);
}
break;     //end of case: "counter-boring"

....

default:    // if does not match any other function then do what is in case: "default"
expandCyclePoint(x, y, z);

[Anonymous]

Thanks. I'm not sure I follow. Do I replace the gCycleModal.format(81) with default?

I have also just noticed another bizarre thing. The beginning of each canned drilling cycle has the tool rapiding back and forth between Z15 and Z5. It also calls out G0 twice in a row. Here is a normal drilling cycle:

N125 M1
N126 T0303
N127 G54
N128 G98
N129 G97 S2950 M3
N130 G0 X0. Z15.
N131 G0 Z5.
N132 Z15.
N133 Z5.
N134 G81 X0. Z-16. R3.75 F48.
N135 G800
N136 Z15.
N137 T0000
N138 G53 X0. Z0.

[Anonymous]

Ah. Just tried deleting the case statement for G81 drilling and posting and that has worked to make the cycle start using G01 X & Z commands instead. So that was easy enough.

I'm still befuddled over the Z15 Z5 Z15 Z5 bit, which is still present. I don't see what's causing that.