Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

5 axis post processor for HY 6040 5 axis mill

19 REPLIES 19
Reply
Message 1 of 20
japmaco
1641 Views, 19 Replies

5 axis post processor for HY 6040 5 axis mill

Was wondering if someone have the post processor file needed for Fusion 360 to able to use the famous Chinacnczone 5 axis HY 6040 cnc mill?

 

Happy new years!

19 REPLIES 19
Message 2 of 20
seth.madore
in reply to: japmaco

What does this machine use for a controller? While we don't likely have a post processor "ready to go", we can guide you to one that is close and provide some assistance in getting things operational. Do you have any sample g-code for this machine?
Adding 5 axis capability to a post is a relatively easy thing to do.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 20
japmaco
in reply to: seth.madore

Hi,

 

This is a link to some g code of the machine

 

https://1drv.ms/u/s!AgVMgapiFJvP0Gao2cqWOCqSfGCm?e=6JIYAF

 

Not sure about type of controller. Will check with the maker. Its running Mach 3

Message 4 of 20

Hi Seth,

 

I have the same machine at home but the 3 axis version, it's a small cnc engraver, mainly meant to cut wood, plastic or if you are not on a hurry, aluminum.  It runs on mach3 which means doesn't have any RTCP or 5 axis tool comp.  Everything has to be handled by the post.

 



Michael Grenier
Senior Solution Engineer
Message 5 of 20

https://www.chinacnczone.com/en/new-desktop-mini-5-axis-cnc-milling-machine-hy-6040-from-chinacnczon...

 

Im using this machine.

Cuts alu like butter... But i have to double check the controller. 

Message 6 of 20
japmaco
in reply to: seth.madore

This is the general mach3 processor used. 

How much work is it to add the 2 axis missing?

 

Would be happy if someone could help me out or guide me in the right direction. 

Message 7 of 20
seth.madore
in reply to: japmaco

Adding 5 axis control to a post can be done through these steps:

https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/sfdcarticles/sfdcarticles/How-t...


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 8 of 20
dan3s2020
in reply to: seth.madore

Hi! I managed to get my hands on a postprocessor for this machine, but I have a problem

 

I set XY0Z0 at the intersection point of the 4th and 5th axis

IMG-20220729-WA0002.jpg

I placed my stock of 60x55x95mm and moved the tool on top of it

IMG_20220801_083211.jpg

So I've made this stock on Fusion360 and created a origin point that is 52mm from the top.  

I use face operation to make my stock 50x50x95, the orientation and movements of the 4th and 5th axis looks fine but my Z goes too deep into the material 

IMG_20220730_165746.jpg

Screenshot_20220801_085141.jpg

 

 

I can see that the postprocessor has a fixed setting "pivotDistance" set to 25mm for reasons I don't know, but if I change it, it changes the Z values. 

 

I have to mention that I do have this  f3d and postprocessor from the seller, that I tried and worked fine, or that was my first impression... 

 

What do you think I'm doing wrong? 

 

Message 9 of 20
CNC_Lee
in reply to: dan3s2020

If you upload the file and post, I will take a look and see if I can help solve this issue.

If my post answers your question, please use Accept as Solution.

CNC Lee
Fusion 360 CAM Post Processor Expert
https://linktr.ee/cnclee
Message 10 of 20
CNC_Lee
in reply to: japmaco

I assume the tool length and WCS values are set correctly?

 

If my post answers your question, please use Accept as Solution.

CNC Lee
Fusion 360 CAM Post Processor Expert
https://linktr.ee/cnclee
Message 11 of 20
dan3s2020
in reply to: CNC_Lee

"I assume the tool length and WCS values are set correctly?" 
i really don't know..? I haven't used tool length on 3 axis so i assumed that it is an option only for ATC .... I'm not sure about WCS...

I'll attach the f3d files and postprocessor, thank you for your time

Message 12 of 20
dan3s2020
in reply to: CNC_Lee

Here i uploaded a short video with the model from the seller working fine on the machine

Message 13 of 20
dan3s2020
in reply to: CNC_Lee

Any thoughts?

Message 14 of 20
paulHNYKH
in reply to: japmaco

I also have one of these HY-6040 5 axis mills. From what I can see the Mach3 controller is a Fly Motion T6C. 
Does anyone know what post processor will suit this?
Thanks in advance 🙂 

Message 15 of 20
engineguy
in reply to: paulHNYKH

@paulHNYKH 

 

Mach3 is the control software, so that is the Post Processor that is required, there is a 5 axis PP that was done a while back specifically for Mach3 and has worked well for a number of people 🙂 Latest version downloaded and attached for you below.

 

It is currently configured for B and C axis which should be the way your CNC is configured, if not then it can be easily modified to suit your configuration 🙂

Message 16 of 20
engineguy
in reply to: engineguy

@paulHNYKH 

 

This may or may not be of help to you, see image below for modelled HY6040 Trunnion and attached Fusion file, used with the 5axismaker PP should work 🙂

 

HY6040-5-Axis.jpg

 

Message 17 of 20
paulHNYKH
in reply to: engineguy

That's so cool Thank you Rob!
Message 18 of 20
gd9606
in reply to: engineguy

Hi, 

thank you very much for sharing the post processor. 🙂  I tried to use it on my HY6040 but I have some understanding problems with it. 

My machine is configurated in x,y,z and B rotates around x and A rotates around z.

For this I tried to edit the post processor: 

gd9606_0-1676825674424.png

 

I put the wcs at the intersection point of the A and B - axis. Because of this I thought I can neglect the pivotDistance and cAxisOffset. Is that right or for what are these distances?

gd9606_1-1676825892066.png

 

I tried to test the 3+2 Axis function with the following part:

gd9606_2-1676828688952.png

 

But if we look now to the g-code i noticed some problems:

The first planing operation should be correct because the block is 50 mm high and wcs is 14 mm away from the bottom so the z value should be 36, which it is:

gd9606_3-1676829085451.png

 

But at the third operation - the pocket - there is a problem I guess. The block is 30 mm thick and the pocket is 1 mm deep, so the z value should be 14mm, or am I wrong? Here the z is 2.97 and that is to low I think.

 

gd9606_4-1676829326814.png

 With changing of the pivot distance the z value changes. So I think this error is pretty similar to the error @dan3s2020 had with his post processor. But I wasn't able to find a solution by myself. 

 

I would be very thankful for any thoughts or help.

 

Best regards

David

 

 

 

Message 19 of 20
engineguy
in reply to: gd9606

@gd9606 

 

 

Apologies for the delay responding, needed to spend some time getting my head around this layout and creating some Models for the HY6040 CNC.

 

I have done a Video that I hope will be of some help, it is done assuming that you have the B and A axis correctly setup at the CNC, if it is as per the setup I have used in the representation of the Trunnion then using a G54 WCS Offset in Fusion if you set the G54 Work Offset in your CNC Control to for example the Top/Front corner of your piece of Stock then the control should execute the G Code in the correct location with reference to your B and A axis  machine Zero.

As I don`t have an actual CNC with the same physical layout I can`t properly test the G Code so I will  have to leave that to you to test (Very carefully) at the CNC, hope all this is of some help to you 🙂

Regards

Rob

Message 20 of 20
gd9606
in reply to: engineguy

Hi Rob,

thank you very much for your response and all your effort, that’s really amazing. 😊
I tried the post processor today and it worked fine for 3 + 2 axis milling, thank you so much, you helped me really a lot.
I also tried a simple 5 axis simultaneous part and at first it didn’t work well. But then I changed the “optimzeMachineAngels2” to one because I have read in the forum that mach 3 doesn’t support TCP.

gd9606_1-1677092418179.png


With that change it worked but the movement sounded and looked not very continues. It seemed like the steps were bigger than usual. Do you know if that can happen because of deactivating TCP-mode or is that normal?
Again thank you very much.
Best greetings
David

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums