Mach3 5 axes

[Anonymous]

Hi ,

I'm try to using 5 axes in Mach3 but the post processor is for 3 axes only,

is there any way to modify the post processor?

Any help greatly appreciated!

[skidsolo · Accepted solution]

Inside the post processor look for a section that looks like this :

function onOpen() {

  if (true) {
    var aAxis = createAxis({coordinate:0, table:true, axis:[-1, 0, 0], cyclic:true});
    var bAxis = createAxis({coordinate:1, table:true, axis:[0, 0, -1], cyclic:true});

    machineConfiguration = new MachineConfiguration(aAxis,bAxis);

    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(1); // map tip mode
  }

Yours probably starts with if (false) change it to true whivh will enable the code in between the { }.

Now you can define the rotary axis for your machine. Here is a description of the parameters:

The supported specifiers are:
1.actuator: Specifies that the actuator type (ie. either "linear" or "rotational"). The default is "rotational".
2.table: Specifies that the axis is located in the table or the head. The default is true for table.
3.axis: Specifies the axis vector as a 3-element array (e.g. "[0, 0, 1]"). This specifier is required.
4.offset: Specifies the axis offset as a 3-element array (e.g. "[0, 0, 25]"). The default is [0, 0, 0].
5.coordinate: Specifies the coordinate used in the ABC vectors (ie. "X", "Y", or "Z"). This specifier is required.
6.cyclic: Specifies that the axis is cyclic. Only supported for rotational axes. Only used when a range is specified. The default is false.
7.range: Specifies the angular range for the axis in degrees as a 2-element array (e.g. "[-120, 120]"). You can also specify a single number to create an axis for an aggregate. The default is unbound.
8.preference: Specifies the preferred angles (-1:negative angles, 0:don't care, and 1:positive angles). The default is don't care.
9.resolution: Specifies the resolution. In degrees for rotational actuator. The default is 0.
Parameters
specifiers The axis specifiers. 
Example:
var bAxis = createAxis({coordinate:1, table:true, axis:[0, 1, 0], range:[-120,120], preference:1});
var cAxis = createAxis({coordinate:2, table:true, axis:[0, 0, 1], range:[-999.999,999.999]});

[Anonymous]

I have tried this solution and in partially worked.. instead of generating smooth uniform tool paths similar to those generated in Inventor HSM or fusion 360, it produces deformed and eccentric paths that are far from being OK. Really we (Mach3Mill) users need a reliable Post Processor From Autodesk. Regards

[George-Roberts]

In what way are they deformed? Would you mind sharing an example?

I've worked on many 5x Mach3 posts and all of them are very different. Due to the nature of the Mach3 control, I think Autodesk would find it difficult to make a 'generic' 5x post.

[Anonymous]

Hi George-Roberts,

I've attached 2 pictures in my previous comment that shows the deformation of processed output in Inventor HSM Editor V. 6.2. I attached a .tap file of the output g code here..

Also I have tried to use Fanuc Generic PP. It generates a uniform paths when viewed in Inventor HSM Editor V. 6.2. I noticed that Fanuc output in dealing with IJK for tool orientation.. but there is a strange issue in this that can be shown in the next 2 images:

you can recognise that there are tilt and turn angles in Inventor simulator, but in fanuc output there are just IJK and they are completely ignored by the Inventor HSM editor 6.2 backplot window simulator and the tool center contact point and centerline is always normal to XY plane. And this makes tool body to interfere with the piece.. 

when I open the output .nc file in Mach3Mill there will be an error that Mach3 Cannot read a code that appears in 2 lines which is Started with G43.5 that can't be recognised by Mach3mill (G43.5 Z15. H24). When I deleted this code lines in loaded noramly to mach3mill but still cannot read IJK nor tilting or turn the tool according to IJK values.

I attached the output file of Fanuc .nc for the same process..

[Laurens-3DTechDraw]

Just loaded the .nc file into the HSMEdit. And hit backplot.

Looks great.

Can you attach your current post processor so we can see how you set-up the 5-axis configuration?

[Anonymous]

Fanuc PP is attached here... 

I have the same output toolpath.. but try to run it.. you will see that there is no tool tilt and IJK values are not read in there specified fields. and you will notice that tool is not tilted nor swept according to IJK values... the same is in Mach3mill. and as indicated in the following image:

[Laurens-3DTechDraw]

Actually it does work.

See this video:

Can you attach you MACH3 post? I think we have to setup the machine correctly to get G43.4 which MACH should understand.

[Anonymous]

Here I attached the Original Mach3 that is coming by default with Inventor HSM (only XYZ). and the Multi axis one that I download from this forum with name (mach3mill X axis A and B.cps) this one is showing deformed toolpaths that are from from fanuc one. 

What is required is that (mach3mill X axis A and B.cps) is supposed to behave just like what fanuc does in the HSM editor. 

how can we get Fanuc Generic PP outputs to work on Mach3Mill ? because when I delete this G43.5 Z15. H24 from the nc file it loaded normally but with no tool tilt or sweep because it cannot get ABC angles to output to the machine..

[Laurens-3DTechDraw]

Can you show a picture/sketch of your machine with the axis?

Because table-table A and B axis isn't something that I think would be possible to the usual standards.

But with mach3 you can make anything ofcourse.

[Anonymous]

[Anonymous]

Also I modified the Mach3mill PP file for A&C axis rather than A&B. Result was better a little bit but toolpath deformation of multi axis still there with less eccentricities. attached here..

[Anonymous]

take into account that A is ranged from -90 to 90.. 

[Anonymous]

I noticed that when increasing tilt and/or sweep angle, of 5 axis toolpath will be more deformed and more eccentric... It is ODD because XYZ values must be independent of ABC values.. I think we have to find this in Post processor.. 

[Laurens-3DTechDraw]

I think you will keep seeing deformation in the backplot. Because your machine doesn't support tcp.

I think the code will look weird in the backplot but should be good in the machine.

[Anonymous]

plot is weird in Backplot and Mach3mill display too.. that's I don't run any code like this in my cnc for not to get it damaged..

[Laurens-3DTechDraw]

I think you should run it really slow.

It's the only way to find out if it works. 

[richpicture]

I have exactly the same issues - My Mach 3 machine has the same A and B axis configuration. Posts generated using the HSM A + B pp produces very incorrect paths with TCP on or off. The paths even cross over across the component, these occur as we pass through B zero and rewinds are not handled.

I have tried adding in rewind code etc from the generic Hass 750 with TCP on and off; this addresses the crossed toolpaths but produces very incorrect A and B values.    

I have tried numerous Mach3 pp files from google searches but all to no avail - We really need a Mach 3 Multi axis post from AutoCAD  

This really needs to be addressed by AutoCAD or users WILL drift away

  

[Laurens-3DTechDraw]

AutoCAD doesn't make toolpaths.

So not sure what you are saying here.

[Anonymous]

I am new to this forum, I have the exact same machine, ChinaZone HY6040 5Axis.

I have been a SolidWorks/ CamWorks user for 3 years, I made a Mach3 5 axis post for CamWorks where it has the A axis offset at 17.3mm for this machine.

A tilt is set at -120° to 120° to help reach tight back angles.

I am now trying to make one for HSMWorks. but hear NotePad++ is the way to go?

I have UPG editor but it is for Camworks, not sure what file extensions it will generate.

I too am stuck for a while....