4th Axis fails to post on Tormach

[ACMEracer]

I'm having problems getting a 4 axis tool path to post for my Tormach.

If there is no A axis rotation I'm able to get the tool path to post.  As soon as I set a new tool orientation the post fails and it looks like it's not turning the A axis to the new orientation.

I think I have the setup and contour WCS set properly and I do get the correct result in simulation.

Please see the attached file. (shortened tool path to make troubleshooting easier)

[ACMEracer]

Now that I found the log file it looks like the "direction is not supported for machine configuration."  The post has an input for the 4th axis and I've selected the proper orientation.  Is there something more I need to do?  Is there a way to configure the orientation of the axis for the machine?

[Anonymous]

I changed X and Z axis orientation in setup and changed tool number to 1, posts fine with Haas 4 axis mill.

[engineguy]

@ACMEracer 

What Post Processor are you using, like Vic @Anonymous  I am not having a problem posting code with the A axis set to rotate around the X axis using the Tormach Path Pilot processor, what Vic has posted should be working for you 🙂

If you are using the Tormach Path Pilot PP then open it in Visual Studio/Notepad or similar Text Editot and look for the Machine Configuration area which should look like this, around Line 233 :-

// Define Master (carrier) axis
masterAxis = Math.abs(rotary) - 1;
if (masterAxis >= 0) {
var rotaryVector = [0, 0, 0];
rotaryVector[masterAxis] = rotary/Math.abs(rotary);
var aAxis = createAxis({coordinate:0, table:true, axis:rotaryVector, cyclic:true, preference:0});
machineConfiguration = new MachineConfiguration(aAxis);

The above is a straight copy out of the PP I used and works perfectly 🙂 🙂 🙂

Path Pilot PP attached

Stay Safe

Regards

Rob

[Anonymous]

Using post from HSM library I get this.

[ACMEracer]

After a bit of back and forth on Facebook we were able to sort things out.  I haven't verified yet but it looks like the latest Pathpilot post for Tormach in Fusion will work.  You should just need to turn on the axis by setting it's orientation.

What was the problem?  Well, depending on how you select the axes it will bomb during post.  As was posted above, selecting the axes in a different way can result in either failing to post or posting out without issue.  So far, I've had less failures by selecting X and Y followed by my box/part point to place the work offset origin.

I'm going to play with it a bit later today or tomorrow and once I figure it out I'll probably start a bug post.  

Also, I ended up with the Xoomspeed post (adds more WCS capability and adds probing).  Special thanks to David Loomes for adding capability to the post.  He also makes a wireless set-up so you can do completely hands off probing.

[Anonymous · Accepted solution]

Initial error I got from your file was "tool length out of range", I renamed tool to #1.

Next error was "Machine orientation not supported", I selected X and Z axis orientation so that Z axis is in line with slot rather then being between two slots as in your original file.

As for axis pointing in other directions, each axis of triad needs to point towards positive side of each axis in the machine, other arrangement can produce code but code will not be in sink with axis of machine and you will get weird motions resulting in crash, scrapped part or both.

[Anonymous]

---

@ACMEracer wrote:

After a bit of back and forth on Facebook we were able to sort things out.  I haven't verified yet but it looks like the latest Pathpilot post for Tormach in Fusion will work.  You should just need to turn on the axis by setting it's orientation.

What was the problem?  Well, depending on how you select the axes it will bomb during post.  As was posted above, selecting the axes in a different way can result in either failing to post or posting out without issue.  So far, I've had less failures by selecting X and Y followed by my box/part point to place the work offset origin.

I'm going to play with it a bit later today or tomorrow and once I figure it out I'll probably start a bug post.  

Also, I ended up with the Xoomspeed post (adds more WCS capability and adds probing).  Special thanks to David Loomes for adding capability to the post.  He also makes a wireless set-up so you can do completely hands off probing.

---

Message 5 of 7 above,........ I don't see a problem, do you?

[engineguy]

@ACMEracer 

There is no "Bug" in the software, other than the one on the Keyboard. 🙂 🙂

Just need to learn how things work in the wonderful world of CNC, first the Post Processor has to be correctly configured for the direction(s) required for the machine, axis configurartion goes as follows, normally:-

A axis rotates around the X axis

B axis rotates around the Y axis

C axis rotates around the Z axis

Not hard and fast rules for sure but it does apply to the majority of multi axis setups.

You wanted to have an A axis but you created your model on the Y axis so things had to be shifted around at the Setup stage in Manufacture resulting in X and Y axis being swapped around by Vic and myself.

Tip, always try to workout before hand just how the actual 4th axis and parts are placed in the machine, makes it easier later on 🙂

Just changing the "Rotary table axis" doesn`t mean that the Post Processor will be reconfigured, would be nice to have that, what does have to match up is your Setup, if, as you originally had your model set in the Y axis then the Y axis needs to be selected at point of posting where you select the "Rotary table axis" and of course it needs to match up with how you have actually placed stuf on your table in order for it to machine in the right place.

That`s the rule, whatever axis you have selected to rotate around in your Manufacture Setup that`s the one you need to select at the "Rotary table axis" option at point of posting, just keep them all the same 🙂 🙂 🙂

Hope that helps

Stay Safe

Regards

Rob

[daniel_lyall · Accepted solution]

You just need to make sure the setup is in line with where the first toolpath is going to be and do it every time you do any setup.

[ACMEracer]

I understand a bit better now.  

"You just need to make sure the setup is in line with where the first toolpath is going to be and do it every time you do any setup."

This would have been a much easier explanation.  It's important to simplify the basics a bit as not everyone is a machinist.