4-Axis machining - post

[Anonymous]

Hi,

I have just started playing with 4-axis machining. I use "Tool orientation" but there is no "A" positioning posted by postprocessor.

Do I have to configure post? How the post knows which is rotary axis or machine configuration?

Thanks

Marek 

[daniel_lyall]

yes the 4th axis needs turned on what post are you useing.

How to do it is here or let us know what post you are useing and it could be done for you

https://forums.autodesk.com/t5/hsm-post-processor-forum/how-to-set-up-a-4-5-axis-machine-configurati...

[Anonymous]

Daniel,

I am using Fanuc generic. I cannot find all the settings described in the link you have directed me to.

The post gives me only G68.2 X0. Y0. Z0. I0. J90. K0. except A or B axis rotation.

[daniel_lyall]

Did you get that post off the post page ( from here http://cam.autodesk.com/posts/ ) or out of fusion in the use generic post 

If you did get it from the use generic posts have you tried the one highlighted.

the generic fanuc post with the 4th turned on is in the zip folder that's attached  

[Anonymous]

Daniel,

I have tried fanuc.cps-Generic Fanuc. Will try inverse time you have attached.

Thanks

Marek

[Anonymous]

Daniel,

I have downloaded fanuc inverse feed from the link and it works after the changes.  I have also downloaded yours (from the zip file) but I cannot make it works.

It does not generate any 'A' code.

This is what I have changed.

  if (true) { // note: setup your machine here
    var aAxis = createAxis({coordinate:0, table:true, axis:[1, 0, 0], range:[-360, 360], preference:1});
    //var cAxis = createAxis({coordinate:2, table:false, axis:[0, 0, 1], range:[-360, 360], preference:1});
//    machineConfiguration = new MachineConfiguration(aAxis/*, cAxis*/);
    machineConfiguration = new MachineConfiguration(aAxis);

[daniel_lyall]

It worked for me can you post a file you are try to output A axis moves on

[Anonymous]

Daniel,

I am new t this forum, and I am not sure what are you asking me for. Do you want me to attach fusion file or posted NC code?

Thanks

Marek

[ivan.stanojevic]

@Anonymous Please post your file.

[Anonymous]

Here are attached both files.

[daniel_lyall]

It seems the fanuc.cps-Generic Fanuc does not like indexing with the 4th turned on.

If the Generic FANUC - Inverse Time and A-axis worked just use that.

Just one thing on your file what direction is the 4th axis facing is it on the left side of the machine facing in the X+ direction or on the right side facing in the X- direction. this is a important question you may have the X axis pointing in the wrong direction what is just flip direction to fix.

[Anonymous]

Daniel,

The chuck holds part  at the right side, all machined material is at X+ side.

[daniel_lyall]

---

@Anonymous wrote:

Daniel,

The chuck holds part  at the right side, all machined material is at X+ side.

---

You do have it around the wrong way this Gcode sample is from your file 

X-0.284 Y-0.3893 Z0.7736
X-0.2831 Y-0.3895 Z0.7698
X-0.2816 Y-0.3899 Z0.7662
X-0.2796 Y-0.3904 Z0.7628
X-0.2772 Y-0.391 Z0.7598
X-0.2743 Y-0.3918 Z0.7573
X-0.271 Y-0.3926 Z0.7552
X-0.2675 Y-0.3935 Z0.7537
X-0.2638 Y-0.3945 Z0.7528
X-0.2601 Y-0.3954 Z0.7525

This bit is if you just flip the the X axis and keep the origin at the same end as it is now It's setting your X, Y and Z zero at dead center 4th axis end of the model how you have it now.

X0.284 Y0.3893 Z0.7736
X0.2831 Y0.3895 Z0.7698
X0.2816 Y0.3899 Z0.7662
X0.2796 Y0.3904 Z0.7628
X0.2772 Y0.391 Z0.7598
X0.2743 Y0.3918 Z0.7573
X0.271 Y0.3926 Z0.7552
X0.2675 Y0.3935 Z0.7537
X0.2638 Y0.3945 Z0.7528
X0.2601 Y0.3954 Z0.7525

[Anonymous]

Daniel,

I think it is OK.  Chuck is at X+ side. The first lines of  X negative values are because tool starts  at the left side from the part. If you take a look later in the nc code it is moving towar X+.

Do you know how to program this part in Fusion and set Z0 at the top of OD diameter?  Right now Z0 is set at the center of rotation. Sometimes I have to set Z0 at the top.

[daniel_lyall]

If it sits in the machine like that pick it's fine then, I went by what I could see in front of me.

I have always been told to do it at the dead center, this is by guys that have 30 plus years.

[Anonymous]

The dead center is on the left side, chuck (indexer) is on the right side. All our vertical mill  machines have indexer at right side. Live center (we call it tail stock) if needed is at the left side.

Thanks

Marek

[daniel_lyall]

I will have a play soon and see if I can come up with something, with or without a pattern, it may just be that you cant use a pattern.

[daniel_lyall]

Would a index with the toolpath oragin at the top with the setup at dead center work for you, this works how well not sure yet

[Anonymous]

Daniel,

I made fanuc generic post work with 4-th axis.

There is one more line 

var forceMultiAxisIndexing = false; // force multi-axis indexing for 3D programs

Once I have changed it to "true"- it works.

Marek

[daniel_lyall · Accepted solution]

@Anonymous

Here's the good and bad news If when you do the setup and have the origin at dead front or back center, then do the toolpath with it's origin where you wont it to be, then do the pattern and select the edge it works.

So that's how you do it.