Help enabling 5 Axis on mach3 postprocessor

[Anonymous]

Hello, I am new to fusion 360 as well as Manufacturing.

What I need is:

*To modify the post processor to activate A and B axis (A is mounted in Z axis and B is mounted in Axis).

*Give the limits of A and B {(A will be -180,180)(B needs to be -120,120 )[I use 0 as center]}

*To make sure the Machinning limits don't exceed the soft limits of my machine.

*That the mach3 software tool path shows the right path.

What I'v been doing so far:

I have a no brand CNC 5Axis Machine. I've been using mach 3 post processor with 3 axis (XYZ) and works just fantastic, The problem is when I try to run the 2 extra axis (A and B-head to head-).

I have been doing research and learning about rewriting the post processor, I have also been reading all over the place and I could not figure out how to do it right. So far I can make it move the 5 axis at the same time but does not follow the specific path. In mach3 software it shows the right path but when I execute the program on my CNC machine it does not respond correctly. I am running out of ideas of how to modify the program so some assistance will be really appreciated.

I have been following step by step the forums but no luck so far with modifying the post processor.

The main post processor for my CNC

for the 3axis, I use "mach3mill" (Which I try to modify with no success).

The one I found (in fusion360 forums)for the 5axis is "mach3mill X axis A and B" but this does not work right (I been trying to modify with no success).

The most resent I've been trying is the "Current progress 5axismaker1" I did modification on my program mach3 software (Using A as C axis).

Thank you in advance!

[engineguy]

@Anonymous 

Just looking at your video it looks as though from the angle of the camera that the B axis is in reverse, the cutter should be pointing in the opposite direction towards the imaginery block on the bed so I think the B-45 should be B45 maybe ??

P.S. If as @daniel_lyall says you can zip your Mach3 XML file he (Or anyone with Mach3) can run the code to check for errors in order to help you more 🙂

Regards

Rob

[Anonymous]

Hello @daniel_lyall 

Thank you your suggestion. I will attach it now hopefully is useful to @boopathi.sivakumar 

[Anonymous]

I know I saw that to. So far it seems that @boopathi.sivakumar set it up right the post processor just it needs to be configure right to optimized the experiences with fusion 360. I try to manually modify the path and look better, however, when I have a complex shape, will be impossible to modify by hand, that the whole reason of fusion 360! I love it.

Thank you for you suggestion. I update the mach3 file settings!

[boopathi.sivakumar]

@Anonymous 

Now the angles are coming out fine as expected but the problem is the machine is not having any RTCP i think so it is not compensating for the rotation.

In other machine if it has RTCP then it uses G43.4 (for Fanuc ) to compensate the rotation moves it will taken care by the controller itself. But if the machine doesn't support RTCP then it has to be compensate in the post processor by adding the pivot distance and the tool length, 

 

It requires lot of testing and back and forth work to modify the post which support for this kind machines and unluckily your machine falls under this category,

I will suggest you to contact one our service provider near by your place,they will help you out on this.

[engineguy]

@cuan_cuan 

Here is a setup that does work here, whether it is of any use to you then you are welcome to use it.

I have used a 6 axis Mach3 setup and I am using the A and C axis as that is what I think should be the correct setup for a "Tilting Head" machine which is what you appear to have.

All the files I have used I will attach below and for your information the version of Mach3 used is 3.043.062 and it seems to be stable enough.

Below is a short section of the code being run, it is quite a long program so I only did a small part of it otherwise it would have been a very long video !!

I can only attach 3 files so I will put them in another post.

Hope it is of some use to you 🙂

Regards

Rob

[engineguy]

@Anonymous 

Here is the other file you need.

It works on screen OK but I don`t have a machine setup to run the code on so I will have to leave that to you!!

As @boopathi.sivakumar  rightly points out you will have to be very careful regarding the tool clearance when rotational rapid moves are made, so have a go with all the stuff I am sending you, worth a try, you will have to re-connect your current B axis motor drive at your Breakout board to the C axis output and because that is how I have it running.

Post Processor and the G code files attached below.

Regards

Rob

[daniel_lyall]

Mach3 in most cases does not play nicely with 5 axis machining, a few guys have made there own program to run the G code through first.

Have a look on the mach3 forum and ask there about 5 axis stuff as well. 

[engineguy]

@daniel_lyall 

Well, it does appear to be running the code through my Mach3 setup here, granted I don`t have a machine hooked up to it but with the right hardware I see no reason why what I have now with possibly a few "tweaks" wouldn`t work with a mechanical setup as per @Anonymous machine, it is a fairly straight forward tilting head A and C axis from what I can see.

One of the biggest issues with multi axis machining is trying to keep all the 5 axis in syncronisation, without pretty good hardware and a system where all the motors have Encoders that feed back to the actual motion controller, without that you are just continually "chasing your tail", believe me I know how frustrating it can be, I have never seen it done successfully using Stepper motors and low quality motion control hardware !!

Long story short, I retrofitted small VMC for a friend (We were nearly not friends by the end) and tried all sorts of stuff but nothing worked as we wanted, finally ended up putting some Mitsubishi servos in place of the Steppers, A much bigger Yaskawa Servo for the spindle motor, an 8 axis Gallil motion control board. All top quality equipment and once we got the hang of programming the Gallil motion controller it worked like a dream, that was around 5 years ago and it is still running as accurately today.

A small Trunnion type 4/5 axis unit was fitted and tested and that worked first time except for the trunnion swinging outwards instead of backwards, a few clicks to reverse the motion and all done. Because all the motors including the spindle motor had Encoders that were fed right back to the Gallil controller and not just to their drives in a "closed loop" system it also meant that not only was the Gallil able to adjust everything instantly and because the spindle had an encoder the machine would do a proper G84 tapping cycle ridgid tapping !!

I do have some motors and drives down the workshop so I might get off my rear and have a go at building something again, bit rusty but hopefully it will come back to me, trouble is it is getting a bit cold down there now, second thoughts, I might leave it till the Spring 🙂 🙂

Regards

Rob

[daniel_lyall]

Yer if you have the right setup it does work and indexing works fine my little 3 axis machine running mach3 runs like a dream I will only change the control if I have no other option.

Artsoft should remove Mach3 since it is a dead product.

[Anonymous]

All right @boopathi.sivakumar, Thank so much for showing me the path to fallow.

[Anonymous]

Hello @engineguy 

Thank you for the time that you take to try to help me.

I am about to try the files that you send me, hopefully will work! I will let you know about the outcome shortly!

[Anonymous]

Hello @daniel_lyall 

Thank you for point me to a direction to go in case I got lost again that probably will happen!

[Anonymous]

Thank you @daniel_lyall  for the inspirational words. as probably you can tell, I am a brand new in the CNC world. But thank's to guys like you, that takes the time to help others is amazing and remains me that still people that are willing to help others with unpriceable knowledge and time with out expecting noting in return. It almost make me cry!

Thank you so much!

[daniel_lyall]

I like helping people I can be very opinionated at times.

If your setup is like what @engineguy  said about what is quite high-end stuff it will be ok you just have to have the right balance.

This is one of 5 axis plugins for M3 here https://www.machsupport.com/forum/index.php?topic=32107.0

[engineguy]

@Anonymous 

I just ran a "Swarf" cut around your block, this has constant movement in both A and C axis so is a pretty good test and I have attached the code below.

Regards

Rob

[Anonymous]

Hello @engineguy I haven run it yet but when i was looking the video, i saw the c value was going to high.

my values are

A axis } -180 to 180 (360)

B axis } -120 to 120 

I am assuming with this configuration

B axis = C axis

now it gives me the problem of the values.

Any how I will set it up and run in  the machine so u can see it in a bit.

Thank  you.

[Anonymous]

Hello @engineguy That post processor will not work in my machine because it does not have a table. I bealive that the Doosan VMC Fanuc machine type is table-table and i have a head-head. I dint run in in the machine because I know is not going to work because I try before. But I will keep learning to edit the postprocessor and you are totally right. out there the is all ready post processor made that i will use to set up my machine. 

Thank you tho and thank for for the screenset!

[daniel_lyall]

it just needs table set to no instead of yes

[engineguy]

@Anonymous 

If it will not work then I must be missing something, it works fine here, the code being produced by the Post Processor I sent you is correct.

I can only think that I have looked at your machine wrong in your Video and am not seeing how it works !!

Here is what I see, bolted to your Z axis rails you have a block with a Stepper motor that spins all the other parts including the Spindle motor around the Z axis, just goes round and round, that is your C axis so that motor at the very top must be connected to your Motion Control hardware C axis output.

Next, lower down you have another Stepper motor that swings your Spindle from left to right about 95 degrees +/- (I can`t tell exactly), that is your A axis and should be connected to the A axis output.

You will need to reconfigure your "Ports and Pins" and enable your C axis and disable your B axis, the XML file that I sent you for the 6 axis screen is already set for C and A axis motors.

I have done another "Swarf" toolpath that goes around a cylinder so that you can see from the code more easily just what is happening.

When you look at your machine from the front I assume that when the machine is at Machine Zero then your spindle is directly in front of you, if this is so and you have re-configured Mach3 as described above then when you go to your MDI and type in G1G90C90F10 then your spindle should move either right or left depending on how you have it set 90 degrees, so it is now to one side as you look at it, now if you type G1G90A-45F10 your A axis with your spindle on it will move from being vertical to a 45 degree angle. That is correct for your machine configuration and that is exactly how the Post Processor is generating code.

Here is the beginning of the code I am  sending you :-

(SWARF2)
N50
N55 T1 M06
N60 S5000 M03
N65 G54
N70 G00 A-45. C90. This is the first move of this program, you can see it is exactly as I have described
N75 G00 X1.6846 Y2.233
N80 G43 Z3.6 H01

Next as the program runs you can see that the A axis stays at the 45 degrees (Or near enough, don`t know why all the tiny differences, might just be tolerance setting) and the C axis changes as it rotates around the Z axis :-

N235 X1.6744 Y1.412 A-45. C87.098
N240 X1.6726 Y1.3834 A-44.997 C86.13
N245 X1.6703 Y1.3548 C85.162
N250 X1.6676 Y1.3263 A-44.998 C84.193
N255 X1.6644 Y1.2978 A-44.999 C83.224
N260 X1.6607 Y1.2693 A-44.998 C82.255
N265 X1.6565 Y1.241 A-44.997 C81.285
N270 X1.6519 Y1.2127 A-44.998 C80.315
N275 X1.6467 Y1.1845 A-45. C79.345
N280 X1.6411 Y1.1564 C78.374
N285 X1.635 Y1.1284 A-44.999 C77.403
N290 X1.6284 Y1.1005 C76.431

All you need to do is re-configure your Mach3 and your physical connections to run a C and A axis system.

Please do this and let us all know how you get on, apart from some very minor "tweaks" to the Post Processor for the Homing at the start and end of the program I reckon it should be fine.

There will obviously be some physical issues with cables going round the axis but if you just program within a 360 degree limit for the C axis and say -95 to +95 in the A axis you should be OK !!

I think that`s all I have for now, hope you can understand what I am trying to do, just need your feedback 🙂 🙂

Regards

Rob

[engineguy]

@daniel_lyall 

No need to change anything table wise in this PP, it is already setup for C and A axis, nice when you get a PP that has about 90+% of things already done, doesn`t happen often 🙂 🙂

Regards

Rob