Post Processor Help

[Anonymous]

Hello, Has anyone worked on a Siemens 840D Post Processor which will work for a 4th A axis? IT is a normal VMC machine with a A-axis on the right side.

Help please?

[Matthew-R]

Hi @Anonymous, thanks for posting on the forum.  Here are a couple of links that you might find useful.

Here's a link the the Siemens post for you to download if you haven't already.

Siemens Sinumerik 840D Post Download

And, here's an article about enabling 4th and 5th Axis on most of the post processors that we have published.

How to set up a 4/5 axis machine configuration

I see that you're new to the forum and I just want to say welcome.  Please reply with any more questions that you have and the community will be here to help you out!

[michaelthompson83]

Hi Matthew can you's add the siemens 840D edditted post for a VMC with a 4th axis mounted on the right hand side to the post library please. I have tried edditting the post but could not get it to work correctly from following the instructions. I managed to find one that some one else had edditted but some of the code was wrong. It worked fine for 3+1 but when i wanted to machine some wrapped geometry it ****ed up. What it cut on the machine was not the same as the simulation. The code had triori and trafoof in it which according to the machine manufacturer it should not be in. The machine is a 1100HD XYZ with an 828D sinumerik control on it

---

[michaelthompson83]

? Can somebody from Autodesk provide a link to how to successfully edit the siemsens post to run on a standard VMC with the 4th axis set up on the right hand side of the table with the centreline of the 4th axis running along the x axis. The same as the Haas 4th axis post. At the moment I have not been able to edit the Siemens 4th axis post successfully. It works for 3+1 but not swarf machining or wrapped contours with the 4th axis moving simultaneously whilst cutting. The code produces a triori code which very few controls accept this. It is some kind of specialised tool point control. Can we have instructions how to turn this off maybe?

[bob.schultz]

The modification to the Siemens' post to support a 4th axis without TRAORI can be easily be done.  You need to modify the code that defines the A-axis in the onOpen function and let the post engine know that TCP or TRAORI is not supported on the machine.  The code should look like the following.

  if (true) {
    var aAxis = createAxis({coordinate:0, table:true, axis:[1, 0, 0], cyclic:true, preference:1});
    machineConfiguration = new MachineConfiguration(aAxis);

    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(1); // disable TRAORI
  }

This should output the coordinates that your machine expects to see.  One issue you may have is with feed rates, since the control does not know where the tool tip is in relationship with the part when TRAORI is not supported.  You will probably have to add inverse time or DPM feed rate support to the post.  You can find out how to accomplish this in the post in the Post Processor Training Guide, in section 7.6 Multi-Axis Feedrates.

[michaelthompson83]

Bob this is starting to take the piss now. I have followed your instructions but the post is still posting the traori code! I have a HNC in mechanical engineering and own one 3rd of a precision engineering firm and I am also an established CNC programmer/ machinist. 

I have even involved one of Autodesk's suggested partners to have them edit the post for us but they seem to be struggling more than what I am as they are even further behind my progress! What a let down to some great software. Why be bias and have a 4th axis Haas generic post which works fine but no standard siemens generic 4th axis post? Do the obvious thing and add the post to the library rather than have people move away from Autodesk products. No wonder Hypermill is becoming so popular despite the price. I have wasted days on this now which is costing us a fortune!

[michaelthompson83]

Also just to point out that the Haas gemetic post does not translate the tool movements from fusion to NC code correctly. Check out the image which i have attached.
Im the simulation the tool path was perfect. When you run the code through the NC plotter it comes up wrong with lines missing and lines added. Considering this is from the Autodesk library it raises some concerns to the safety and ease of edditing these generic post's if you's can not even get this right! This is the 2nd bug that i have came accross with wrapped geometry and engraving around a cyclinder. We are a start uo company so we do not have £18k to spend on a laser etcher with a 4th axis.

[bob.schultz]

Hello Michael,

The example code should have worked for you.  Please make sure that the post optimizes the output coordinates for the table rotation as shown in the code below.

  optimizeMachineAngles2(1); // disable TRAORI

You should also see the following code in the onSection function that will not output the TRAORI command when the above setting is used.

    if (currentSection.getOptimizedTCPMode() == 0) {
      writeBlock("TRAORI");
    }

The onSectionEnd function should have the following code.

  if (currentSection.isMultiAxis() && (currentSection.getOptimizedTCPMode() == 0)) {
    writeBlock("TRAFOOF");
  }

If for some reason your post does not have this code, then download the latest version of the Siemens 840D post processor.  You can also change the conditionals to 'false' so that the TRAORI code would never if for some reason it still does not work.

    if (false) {
      writeBlock("TRAORI");
    }

As far as the tool movements being incorrect, this is addressed in your other forum thread.

https://forums.autodesk.com/t5/fusion-360-computer-aided/engraving-bug-on-wrapped-tool-path/m-p/8209...

[michaelthompson83]

Hi Bob,

For some reason i cannot reply to your email or send a private message. There is an issue with the post that you sent me with the cycle 800 which the control does not except. Can this be turned off? Or is it needed in the current post set up?

[bob.schultz]

The CYCLE800 can be disabled in the Siemens post by making the following change to the post processor.

// fixed settings
var firstFeedParameter = 1;
var useMultiAxisFeatures = false; // set to false

You should now see A-rotations for 3+2 operations instead of the CYCLE800.  It will also get rid of the CYCLE800 block that is cancelling a 3+2 operation as is shown in your picture.

[michaelthompson83]

I now get a "incorrect position programmed for axis/spindle A/MA1" message