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: 

Strange G-code output from Rotary toolpath

16 REPLIES 16
SOLVED
Reply
Message 1 of 17
luke.bladesYS6HE
616 Views, 16 Replies

Strange G-code output from Rotary toolpath

Hi All,

 

I'm trying to run my first rotary toolpaths with a 4th axis i've built recently. The model i've attached is a trial to get things working properly. The toolpath looks fine in simulation (the tool revolves around the work but that's just how fusion represents the 4th axis toolpaths). The problem is when I ran a trial run on the machine, it seems to do something different to the simulation and the Gcode reveals why.

 

Instead of holding the tool relatively still and cutting the helical toolpath with the 4th axis (with small changes in X and Z), the gcode output produces a helical path for the tip of the tool using the Y and Z axes (which would obviously cut right through the work if I ran the code on the machine).  I'm sure i've got something wrong in the setup, but I havn't been able to find what it is. 


Very grateful for any help with this,

 

Luke

Labels (2)
16 REPLIES 16
Message 2 of 17

@luke.bladesYS6HE 

What post processor you are using ? is it a customized one or from the post library?


Boopathi Sivakumar
Senior Technology Consultant

Message 3 of 17

Hi,

 

Hi, thanks for your response. I'm using a customised mach3mill post processor.

 

I managed to figure it out in the end. The issue was that origin had been set to a point that was on along the rotary axis. I changed the origin and the code works fine now.

 

Cheers!


Luke

 

 

Message 4 of 17

Hello,

 

I have an issue about same topic.

I have done the set-up geometry and milling process mutli axe rotary.

 

I select postprocess to Mach3 (rotary in along x axe) and then it results that:

- In the gcode there are too many lines with Y movments.

- Y should be offseted from the center by 5mm and not moving from there.

- When I process it with the machine, it repetes several time the similar operation in the same x (zero) point.

2_ When it starts the gcode (line 79) starts also the spinner movment along the x axe (along the rotary axe) but the  the rotary stops to rotate in one point.

 

Do you know why? Do you know what is the problem?

Message 5 of 17
seth.madore
in reply to: mastro_dan_d

Could you share your Fusion file here?

File > Export > Save to local folder, return to thread and attach the .f3d file in your reply


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 6 of 17
mastro_dan_d
in reply to: seth.madore

Thank you for the fast replay.

 

Here is the file .f3z.

 

I dont have the option .f3m. Is that readable for you?

Message 7 of 17
mastro_dan_d
in reply to: seth.madore

Thank you for the fast replay.



Here is the file .f3z.



I dont have the option .f3m. Is that readable for you?
Message 8 of 17
seth.madore
in reply to: mastro_dan_d

The geometry of the part is simply not going to allow it to stay at Y0, the peaks and valleys are too great to allow that.

 

Does your machine not have a Y axis?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 17
mastro_dan_d
in reply to: seth.madore

I have the Y. 

In the rotary parameters I have placed Y offset 5mm. So the center of the spinner can reach the corners of the geometry.

 

But the gcode Y is not staying in Y 5mm.

This is present in the simulation.

Additionally, in the gcode, in the first part there is not x coordinate.

 

Furthermore, when I run the gcode, 

When it reaches the line 79, the rotary axe X stops to rotate (I have tried to run the code in the machine).

 

 

Message 10 of 17
seth.madore
in reply to: mastro_dan_d

What post processor are you using, and could you share it here? Without that, I can't speak much to what's going on at N79

 

Don't go off the numbers in the Simulation, it has no concept of a rotary axis, so what you see in "Y" is not entirely accurate. That said...

 

In a test with a Haas NGC post (TCP set to OFF), I'm getting values that roughly go from Y4 to Y6.

Using your same toolpath on a perfect cylinder, I'm given a static value of Y5.

I'm highly doubtful that Rotary is just going to lock the tool at that position given the geometry of your part


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 17
mastro_dan_d
in reply to: seth.madore

Here it is:

- post process from Fusion to Mach3 (rotary axe along x).

 

I have linked both the -mach3mill_.cps (in format .txt) and the -Postprocess_error in machine.tap (in format .txt)

 

Thank you for your time @seth.madore !

Message 12 of 17
mastro_dan_d
in reply to: seth.madore

 https://a360.co/3KZaFYk

 

this is the shared file!

 

@seth.madore 

Message 13 of 17

In your Post Process dialog, did you have "Rotary Axis" enabled as shown:

2023-04-25_15h40_36.png


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 14 of 17
mastro_dan_d
in reply to: seth.madore

Yes!

Message 15 of 17
seth.madore
in reply to: mastro_dan_d

I think that the reason it's stopping at line 79 is that it's hit the 360 degree limit of your machine. We need to change the post to be "cyclic", so it rolls over from A360. to A1, 2 etc. 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 16 of 17

But it appears that it's already set as such....

var aAxis = createAxis({coordinate:0, table:true, axis:[(getProperty("fourthAxis") == "x") ? -1 : 0, (getProperty("fourthAxis") == "y") ? -1 : 0, 0], cyclic:true, preference:0, tcp:useTCP});

 

Hmm... 🤔


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 17 of 17
mastro_dan_d
in reply to: seth.madore

Why the just before that there is written:

 

var useTCP = false;

 

what is it about?

 

Sorry for the multiple questions but I do not know where it goes wrong.

 

Also really strange that there are so many lines in the gcode. When I run it in the machine each line takes 10+ seconds to be processed.

 

The toolpath has been settle to "spiral" but just after the line 79 of the gcode, the X appears and it starts to mill moving in spiral (as I said before from the line 79 the machine rotary axe it stops to turn, meanwhile the x is moving "correctly").

 

 

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

Post to forums  

Autodesk Design & Make Report