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

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

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 »

Why make a simple thing so complicated messing with M codes and stuff? Add a P word on the G84 cycle and it's done. I use it since I put my CNCs together with the tormach tension compression chucks and it works flawlessly. Of course it's not the ideal (rigid tapping is) but It works.
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 »

The fact that the machine stops in Z while the spindle is still at full speed or starts in Z before the spindle has started moving can't be fixed by simply pausing at the bottom of the hole. Think about it and perhaps read the thread a little more carefully, then let us know if you still don't get it.
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 »

Muzzer wrote: Mon Apr 05, 2021 10:36 am The fact that the machine stops in Z while the spindle is still at full speed or starts in Z before the spindle has started moving can't be fixed by simply pausing at the bottom of the hole. Think about it and perhaps read the thread a little more carefully, then let us know if you still don't get it.
I made the comment because I use the feature for years with tension compression heads and it works ONLY with the pause. I will try to explain why.

As soon as the Z axis reach the programmed deep the M4 is issued BUT, as the most of our VFDs driven motors, the spindle does not stop immediately so if you do not pause the Z retraction, It will start to pull the TAP up and break it. The pause is there only to account for the spindle inability to stop immediately.
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: Mon Apr 05, 2021 7:54 am Why make a simple thing so complicated messing with M codes and stuff? Add a P word on the G84 cycle and it's done. I use it since I put my CNCs together with the tormach tension compression chucks and it works flawlessly. Of course it's not the ideal (rigid tapping is) but It works.
Why? Because some users do have very customized M3 and M4 macros that they use for normal machine operations that already include dwell commands that would not be compatible with just adding an additional dwell command in Fusion 360 for the tapping cycle.

The solution I posted with replacing the default M3 and M4 command with customized top of tapping cycle and bottom of tapping cycle scripts based on machine parameter 74 and 84 is targeted for those users.

I agree that for most users adding the dwell parameter from Fusion 360 will get the job done.

-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
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 »

swissi wrote: Mon Apr 05, 2021 1:45 pm
rflopes3 wrote: Mon Apr 05, 2021 7:54 am Why make a simple thing so complicated messing with M codes and stuff? Add a P word on the G84 cycle and it's done. I use it since I put my CNCs together with the tormach tension compression chucks and it works flawlessly. Of course it's not the ideal (rigid tapping is) but It works.
Why? Because some users do have very customized M3 and M4 macros that they use for normal machine operations that already include dwell commands that would not be compatible with just adding an additional dwell command in Fusion 360 for the tapping cycle.

The solution I posted with replacing the default M3 and M4 command with customized top of tapping cycle and bottom of tapping cycle scripts based on machine parameter 74 and 84 is targeted for those users.

I agree that for most users adding the dwell parameter from Fusion 360 will get the job done.

-swissi
The goal here is a Cam Post for Fusion 360 right ? So if there is a Dwell parameter on fusion to specify that, the post SHOULD include it. If the user do not want the dwell simply put ZERO on the parameter. Agreed ?
CivilCNC
Posts: 1
Joined: Wed Apr 07, 2021 11:16 am
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: will obtain

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

Post by CivilCNC »

I just have a simple g0704 cnc without a VFD or programmable spindle control. Will this post processor work ok for me? I was having trouble using the one that is integrated in Fusion360.
thanks
Jake
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 »

CivilCNC wrote: Fri Apr 09, 2021 9:55 pm I just have a simple g0704 cnc without a VFD or programmable spindle control. Will this post processor work ok for me? I was having trouble using the one that is integrated in Fusion360.
thanks
Jake
A post processor just creates a M3 or M4 command to start the spindle, a M5 command to stop it and an S... command to set the spindle speed. If you don't have any spindle control wired, those commands are simply ignored and you have to control the spindle speed, start and stop manually.

When you talk about the post processor integrated with Fusion 360, I assume you mean the standard Centroid Mill post processor from the online HSM library, correct? This post processor here is based on the standard post processor and has a lot of additional features added.

If the standard Centroid Mill post processor does not work for you, it's highly likely that you are doing something wrong and I'm not sure that using this one will fix that problem but nobody will stop you to give this one a try.

-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 »

The std G84 canned tapping cycle stops both the downfeed and the spindle at the same time, unless I'm missing something. The down feed on most machines usually stops pretty much immediately, whereas the spindle has to decelerate to a stop. So, as it slows down, the tap continues to pull into the hole. The tension compression head is now in tension (extension). This is the point at which the P pause is activated (again, correct me if I'm wrong). After the pause (if you have it), both the spindle and the up feed are commanded. Again, the up feed happens almost immediately, whereas the spindle takes a while to get up to speed. So the tension compression head comes under even more tension (extension). This can get a bit hairy. Tell me how adding further P pause would have helped? I could increase the pause long enough to go and take a long crap and it wouldn't make the slightest difference to the total extension of the tension compression head at the end of the cycle.

If on the other hand you were to introduce a delay within the M4 macro, you could start the spindle before the up feed and you'd be able to recover some of the tension (extension) before the up feed started, or at least minimise any further extension. That is something you could do quite easily with modified M3/M4 macros but no value of P will ever achieve it.
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 10, 2021 2:09 pm The std G84 canned tapping cycle stops both the downfeed and the spindle at the same time, unless I'm missing something. The down feed on most machines usually stops pretty much immediately, whereas the spindle has to decelerate to a stop. So, as it slows down, the tap continues to pull into the hole. The tension compression head is now in tension (extension). This is the point at which the P pause is activated (again, correct me if I'm wrong). After the pause (if you have it), both the spindle and the up feed are commanded. Again, the up feed happens almost immediately, whereas the spindle takes a while to get up to speed. So the tension compression head comes under even more tension (extension). This can get a bit hairy. Tell me how adding further P pause would have helped? I could increase the pause long enough to go and take a long crap and it wouldn't make the slightest difference to the total extension of the tension compression head at the end of the cycle.

If on the other hand you were to introduce a delay within the M4 macro, you could start the spindle before the up feed and you'd be able to recover some of the tension (extension) before the up feed started, or at least minimise any further extension. That is something you could do quite easily with modified M3/M4 macros but no value of P will ever achieve it.
I haven't tested this myself as I prefer thread milling over tapping but looking at the graphics from the CNC12 Mill User Guide, it looks like the spindle is started in reverse at the bottom and then the P dwell delay occurs before the Z retraction move starts.

tapping.png

Adding the P dwell parameter into the Post Processor output is definitely the right thing to do and it will be included in the next version of the Post Processor. If it's not needed on a machine, it can be set to 0.

The point I was trying to make above, that obviously wasn't clear to all, was: If that dwell parameter P alone does not work for some machines, Machine Parameter 74 and 84 can be used to customize the M3/M4 commands to further fine tune the spindle/Z-Axis synchronization of the G84 tapping cycle.

-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
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 »

YEs that's right. The spindle starts first when the tapping reaches the bottom, that's why the P word is so important for those like me that have just regular motors that cannot simply start/stop immediately. That 0.5s is just what the TC head needs to relief the tension and came out nicely.
Post Reply