Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

swissi
Posts: 471
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by swissi »

ChrisAttebery wrote: Sat Mar 06, 2021 5:58 pm I have a request. At tool changes and at the end of a program I would like to see the spindle shut off BEFORE the final retract in Z.

I'm changing tools manually so I'd like the spindle shut down ASAP when it's done cutting so I can open the door, get my impact wrench lined up, etc. As it is now the machine finishes the final cut, moves to safe Z, then shuts the spindle down.

I've made the changes to my personal copy of the post, but I'd like to see this change made to the newer revisions.
Here's a version that has now a property to turn off the spindle at clearance height together with the coolant. The default of this property is set to turn spindle off, so if somebody prefers the spindle to keep running until the Z-Axis reaches the tool change position, they can turn that property off.

Let me know if that's working for you as expected.


-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
ChrisAttebery
Posts: 78
Joined: Mon Dec 07, 2020 2:20 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 4031
Location: Gilroy, CA
Contact:

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by ChrisAttebery »

I just tried it out. That's exactly what I wanted. Thanks again Swissi.
FlySox
Posts: 46
Joined: Mon Jan 14, 2019 5:57 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by FlySox »

Perfect! This saves me from modifying the post myself; it was my only complaint about this otherwise terrific contribution. Thanks, swissi, and to Chris for the original request.
rflopes3
Posts: 65
Joined: Tue Jan 14, 2020 12:24 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 2752

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by rflopes3 »

Also I would like to see the dwell on tapping cycles.

I do modify the post myself but would be nice to have it by default

the tapping code would be like this:

getCommonCycle(x, y, z, cycle.retract),"P" + secFormat.format(P), feedOutput.format(F)

instead of this

getCommonCycle(x, y, z, cycle.retract), feedOutput.format(F)

The spindle off was a great addition. Thanks.
swissi
Posts: 471
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by swissi »

rflopes3 wrote: Thu Apr 01, 2021 2:51 pm Also I would like to see the dwell on tapping cycles.

I do modify the post myself but would be nice to have it by default

the tapping code would be like this:

getCommonCycle(x, y, z, cycle.retract),"P" + secFormat.format(P), feedOutput.format(F)

instead of this

getCommonCycle(x, y, z, cycle.retract), feedOutput.format(F)

The spindle off was a great addition. Thanks.
Thanks rflopes3, I'll add this to the next version of the Post Processor.

I never used the tapping cycles as I prefer thread milling over tapping and I just noticed last week while helping a supporter with a tapping issue that the post processor did not output the dwell parameter.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Muzzer
Posts: 470
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 38D269594F9C-0110180512
Location: UK
Contact:

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by Muzzer »

That tapping dwell sounds like a great idea. I can't do rigid tapping on my machine because I can't get a spindle encoder on my turret mill and I can't even pick up on the bull gear because CNC12 insists on a silly (>1000) PPR count.

So it means I use a tension compression head but I find the canned tapping cycle starts to retract the tool before the spindle has had a chance to fully come to a stop and reverse direction - thank goodness for tension compression heads! If I understand correctly, this change would pause the retract until the spindle has had a chance to reverse direction - is that correct? If so, that would be very useful.
swissi
Posts: 471
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by swissi »

Muzzer wrote: Sat Apr 03, 2021 7:15 am That tapping dwell sounds like a great idea. I can't do rigid tapping on my machine because I can't get a spindle encoder on my turret mill and I can't even pick up on the bull gear because CNC12 insists on a silly (>1000) PPR count.

So it means I use a tension compression head but I find the canned tapping cycle starts to retract the tool before the spindle has had a chance to fully come to a stop and reverse direction - thank goodness for tension compression heads! If I understand correctly, this change would pause the retract until the spindle has had a chance to reverse direction - is that correct? If so, that would be very useful.
For those without a spindle encoder take note that the CNC12 canned tapping cycle G98 G84 uses machine parameter 74 and 84 to configure the M-Code that's being called on top of the cycle (P74) and on the bottom (P84). By default these parameters are 74=3 and 84=4 so that means on top of the cycle the canned tapping cycle calls M3 and on the bottom M4. As you probably don't want to mess with the M3 and M4 file to add dwell commands that would impact all spindle operations and not just tapping, you could use other unused M commands like M56 and M57 to customize the dwell timing needed for the tapping cycle.

As an example you would set 74=56 and then customize mfunc56.mac to do what's needed on top of the tapping cycle and 84=57 to use mfunc57.mac to handle the bottom.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Muzzer
Posts: 470
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 38D269594F9C-0110180512
Location: UK
Contact:

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by Muzzer »

That's interesting - I must look into that.

The dwell parameters generated by the tap settings in Fusion didn't seem to have any effect - IIRC the CNC12 canned cycle contained a dwell term but I couldn't get it do actually do anything, or perhaps it was dwarfed by the eternity my machine took to come to a stop. In the end I had to reduce the spindle speed as the only means to limit the amount of tension and compression that occurred, as the VFD was already at the max decel possible, even with the rated braking resistor. Sounds as if you may have your finger on it there.

I'd have to think about this, as I'd probably want the tap to start turning CCW before the quill began to rise, to make up for the overshoot it incurred as it came to a stop at the bottom. In the example M57 replacing the stock M4, it would probably amount to an M4 followed by a pause before exiting back to the G84. The complication is that the accel and decel times are very much dependent on the spindle speed to start with, so a fixed pause would still be a bit hit and miss.
swissi
Posts: 471
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by swissi »

Muzzer wrote: Sat Apr 03, 2021 2:12 pm That's interesting - I must look into that.

The dwell parameters generated by the tap settings in Fusion didn't seem to have any effect - IIRC the CNC12 canned cycle contained a dwell term but I couldn't get it do actually do anything, or perhaps it was dwarfed by the eternity my machine took to come to a stop. In the end I had to reduce the spindle speed as the only means to limit the amount of tension and compression that occurred, as the VFD was already at the max decel possible, even with the rated braking resistor. Sounds as if you may have your finger on it there.

I'd have to think about this, as I'd probably want the tap to start turning CCW before the quill began to rise, to make up for the overshoot it incurred as it came to a stop at the bottom. In the example M57 replacing the stock M4, it would probably amount to an M4 followed by a pause before exiting back to the G84. The complication is that the accel and decel times are very much dependent on the spindle speed to start with, so a fixed pause would still be a bit hit and miss.
You could make the dwell time a percentage of the spindle speed to account for different rpms.
Also keep in mind that tapping is a low speed, high torque operation and many spindles have issues with hight torque at low rpms so they might slow down during the tapping process. The feed rate of the Z-axis is calculated from the spindle speed and the pitch of the tread you are tapping. As your spindle doesn't have an encoder, CNC12 would not know that your spindle is slowing down and keeps moving the Z-axis down at the constant feed rate which can create a problem too so you might need to experiment with the feed rate as well.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Muzzer
Posts: 470
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 38D269594F9C-0110180512
Location: UK
Contact:

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

Post by Muzzer »

On my machine, I tap in low speed range - the machine automatically selects low range, given the set speed. Of course, this means the motor is running at a fairly high speed, so still takes a while to ramp down. As you say, the macro assumes that the spindle comes to a sudden stop.

By default, the quill stops descending at the same time as the VFD is told to stop. Then, after the pause (if there actually is one), the quill starts to ascend again. Meanwhile, the spindle has to come to a stop and then start again in reverse. The tension compression head is the answer to this situation but as you can imagine, it can be a bit unnerving.
Post Reply