G93 Support for LinuxCNC

[youcangetme]

Hello!

Since Fusion360 supports Haas it must also support G93 Inverse Timing, right? Is G93 supported with the LinuxCNC post processor as well? $1,500 a year is expensive but if it truly support G93 on LinuxCNC then I will upgrade my subscription.

The thing is I built my own CNC before I had ever used one (or really knew what I was doing) so I built it to be really cool. Full 4 axis in fact. When I was finished to my horror the software to generate true 4 axis motion was 50 times the cost of my mill!

So, my A axis never moves. I still have to home it to get my programs to run though. Every time I home it my heart is saddened that it's been inactive all these years.

Can Fusion360 ultimate actually make G93 Inverse Timing programs for LinuxCNC?

[Steinwerks · Accepted solution]

This is just a post processor function, so yes, there is no issue with posting G93 moves, it just needs to be set up properly.

Please see this thread on setting up a 4- or 5-axis post processor: https://forums.autodesk.com/t5/hsm-post-processor-forum/how-to-set-up-a-4-5-axis-machine-configurati...

[youcangetme]

Thank you, Neal!

I was able to follow the how-to. Problem now is I have to cough up the cash and upgrade!

One more step closer to having a 4 axis machine that actually works!

--jb

[SolidModeling]

Lol... the answer doesn't even answer your question... so I don't know why this is solved!

How do you get the post to convert to G93 and output it... Well I don't think you can do this in fusion mate. Try this guys tool - https://www.ganotechnologies.com/cnc/rapidrotary/

[youcangetme · Accepted solution]

Fusion 360 supports G93, no third party solutions required. Correct, it has nothing to do with post processors.

[SolidModeling]

"Fusion 360 supports G93, no third party solutions required."

Really? How? Where?

How do you set it to output post in G93 and not G94? 

[johnswetz1982]

Like poster above stated, the post processor and control has to support it. Some do not, some do.

[SolidModeling]

It's a pretty simple question which seems pretty hard for anyone to answer...

Linuxcnc 2.7 + supports G93 and the response is Fusion 360 supports G93, but the question is how?

How does Fusion 360 support the output of G33? How do you make it output in this mode to the post file?

[johnswetz1982]

The only 2 Posts processors that I see that support G93 inverse time are Haas and Fanuc. The post for Linux can certainly be modified to output G93 inverse time moves. There is roughly 21 entries that would need to be added/modified. Like what was was stated before is it is just a post processor issue. You can see code posted below that is direct from Fusion thru the Haas inverse time post with no 3rd party program or editor. 

[youcangetme]

I am not sure how much of my setup is customized by the manufacturer but I do use a few profiles they created for me specifically for Mach4 and Fusion 360. Is see where any rotational axis will result in G93.

[SolidModeling]

For G93 their needs to be some calculations done here based on distance traveled and given feed rate. This becomes very trick when you start talking G2 and G3 moves where distance traveled over a radius needs to be calculated.

I think you are talking rubbish re post processor issue. This needs to happen in Fusion 360 surely?

If anyone know how to calculate the distance/length of the radius given R and the start and end co-ordinates please tell me!!!!

[johnswetz1982]

"For G93 their needs to be some calculations done here based on distance traveled and given feed rate. This becomes very trick when you start talking G2 and G3 moves where distance traveled over a radius needs to be calculated."

Fusion does this internally already. Fusion DOES calculate what that would be based on the distance from the center of rotation and the feedrate you program for the operation. I do not think you understand how this works. Fusion generates Machine independent code. A post processor takes that machine independent code and converts/formats it to a machine DEPENDENT code. The post processor is like a magic decoder ring. If your post processor is not set to put out inverse time moves then it will not. But like I pointed out above at least 2 post are set up to do so. 

"I think you are talking rubbish re post processor issue. This needs to happen in Fusion 360 surely?"

This DOES happen in Fusion. You can say that you think its rubbish or that it is not being done internally in Fusion but I already showed you an example of the code posted out and explained that it is a post processor issue so i'm not sure what you need to believe it so. You can even take your model and post out using the Haas or Fanuc inverse time post and see for yourself.

"If anyone know how to calculate the distance/length of the radius given R and the start and end co-ordinates please tell me!!!!"

You dont have to calculate that Fusion does that. That is the point of having a CAM system/software.

[youcangetme]

Huh, turns out that Mach4 is a clone of Func. Imagine that 🙂

[SolidModeling]

"I do not think you understand how this works." Well I didn't; but I understand what you are saying now. Thanks. 

So the real question is who has modified the Linuxcnc post processor to extract G93?

Let me do some study and come back to you.  

[Cris-Ideas]

---

@SolidModeling wrote:

If anyone know how to calculate the distance/length of the radius given R and the start and end co-ordinates please tell me!!!!

---

So ArcLenght=R*angle[rad]

Arc length is directly dependent on radius of the arc and angle of the arc.

If you have radius and start and end coordinated you have all that is required to know the length of the arc.

Use  (x-a)^2+(y-b)^2=R^2 to calculate a & b (coordinates of the centre of the arc).

Once you have those calculate start and end angle

subtract them to get the arc angle

and you have arc length in the next step.

So whether code is outputted in G94 or G93 depends on the post processor solely.

Calculations are pretty easy.

I do not use post-processor but subroutines in linuxcnc that do just that.

BUT:

I have found out a problem with linuxcnc itself when running G93 codes.

Problem is that it does not do it correctly if rotation is the only movement.

So for instance

G93

G1 A360 F1

results in A axis running as G0, so full speed.

but

G1 X1 A360 F1

results in proper interpolation.

Did anyone of you using linuxcnc also have this problem?

Cris.