cant force XZC axis.

[Anonymous]

hi yall,  

I`m using a siemens postprocessing file, now i disabled the Y axis and made sure the usepolarmode is active. 

Now when i export a g-code i still see the Y axis being active... is there some one who really can help me.. i searched all over the place and i just dont get it.. thanks in advance ! 

[Arun.rs]

Hi @Anonymous 

Thanks for raising your concern via Forum.

I believe you are using Siemens Mill Turn Post.  Could you please share the Fusion project? so that I can check and guide you for the same?

Regards

[Anonymous]

No problem i will make a "test" file so we can work on it. 
So this should have the post procces on it aswell. If you have a better program to use for this then use what you think is needed 🙂 

its a lath where we going to convert the X-axis to be able to use a powered mill  on this axis. I try try to convert the Mill axis to fit the X axis but no succes 😞 

[mathew.hutton]

Hi @Anonymous 

I don't think the post get's included if you just export the project, so you'll need to attach the post as an attachment on here. Looking at your project, the way you have the toolpath programmed, it wouldn't be influenced by the "use polarmode" option in the post as polar mode is when the tool is machining in the XY plane, in your case, the toolpath is in the XZ plane. However disabling the Y axis in the post should have worked so there may be an issue with the post.

Cheers

Mat

[Anonymous]

Before you get to post processing, you need to program correct machining process. You used "tool orientation" which wipes out half of the model, you need to use "wrap" function instead and then refine tool path for lead in and lead out, number of passes etc.

[Anonymous]

yea i did this and try many other things i just made the test file so he could look at the post proces but it didnt got send with it. I will make a new post with the post and with the correct file. 

[Anonymous]

post and new version of the part. 

Its simple because i just need to figure out how to make the Y axis not be working.. The C-axis should take care of the Y-axis. 

[Anonymous]

So looking at your first post, you disabled Y axis but you are not saying why you did that. Does your machine have Y axis?

If I relate your sample file with first post and mentioning of polar mode, nothing adds up. Are you machining spiral groove on OD of the stock or doing something on face of the stock because as mentioned above, polar mode only works in XY plane.

Can you upload actual f3d file you are working on ?

[Anonymous]

OK, now we are getting somewhere, this will post in XZC mode,  but I had to suppress manual NC or my post fails.

No idea what "m112" means  but if that was supposed to be G112 (polar coordinate on),..... polar coordinate has nothing to do with cutting spiral grove in XZ plane.

 

[Anonymous]

Ops,.... that's YZ plane, don't need more confusion here. 😁

[Anonymous]

Okee let me explain: 

The lath is converted from manual to cnc. We will use the lath as normal (with cutting tools) but some where in the process we will do a tool change and then in the same holder we will use a mill ( mill will be used on the X axis and the C axis will rotate) 

You can use the X axis to make grooves onthe part.  Thus why I need to lock out the Y-axis. And need to change the post proces to xzc. 

So this will make sure that the Z axis of a normal mill is on my X axis (lathe) and the the mill X axis is my Z axis (lathe). 

And it was a type about my M code it must be G112. Even with this proces it still exporting Y to my gcode. 

I'm sorry for my bad explaining. It's a while ago I use CNC terms and specially trying to explain in English 😅. 

@Anonymous i read some where you need to use G112 to convert Y to X movement. But I suppose I had it wrong. 

I added a photo and you will have a better idea of what I mean with my axis and where my mill will be placed 🙂 

The photo is quickly made, the green line is where the mill will be placed after the tool change. 

[Anonymous]

Forgot the picture hahah 

[Anonymous]

---

@Anonymous wrote:

Okee let me explain: 

The lath is converted from manual to cnc. We will use the lath as normal (with cutting tools) but some where in the process we will do a tool change and then in the same holder we will use a mill ( mill will be used on the X axis and the C axis will rotate) 

You can use the X axis to make grooves onthe part.  Thus why I need to lock out the Y-axis. And need to change the post proces to xzc. 

So this will make sure that the Z axis of a normal mill is on my X axis (lathe) and the the mill X axis is my Z axis (lathe). 

And it was a type about my M code it must be G112. Even with this proces it still exporting Y to my gcode. 

I'm sorry for my bad explaining. It's a while ago I use CNC terms and specially trying to explain in English 😅. 

@Anonymous i read some where you need to use G112 to convert Y to X movement. But I suppose I had it wrong. 

I added a photo and you will have a better idea of what I mean with my axis and where my mill will be placed 🙂 

The photo is quickly made, the green line is where the mill will be placed after the tool change. 

---

Not exactly,..... G112 does not convert Y to X movement.

G112 (polar mode on)

G113 (polar mode off)

Polar mode only works in XY plane  (face of round stock on lathe), it converts Y axis Cartesian coordinate into polar coordinate by means of rotating C axis to angle that coincides with X coordinate of tool position.

Basically works as vertical mill  but, instead of moving Y axis, it rotates C axis which can only rotate around its center axis.

If you have some sort of retrofitted control with custom rotary tool attachment, general principles still apply.

You have to have ability to lock spindle and drive it in increments from  0 - 360  degrees as Z axis is driven from face of stock towards chuck at given pitch.

Mill-turn setup and post should produce the code, you don't need to disable Y axis in post, it will not be used in resulting code unless you use lead in and lead out at angles that would require Y axis moves.

[Anonymous]

no clue what happend.. but some how i got it to work.. this is my code now.

N1(2D CONTOUR2)
M67
G54
G98 G19 M45
G00 G28 H0.
T0202
M08
G97 S12000 M13
G00 C-130.704
G00 Z-3.903
X103.
X83.
G01 X75. F664.76
X53.5
X53.277 Z-3.891 C-130.706 F46.21
X53.066 Z-3.854 C-130.714 F133.59
X52.877 Z-3.795 C-130.727 F211.52
X52.718 Z-3.717 C-130.743 F277.23
X52.599 Z-3.623 C-130.763 F328.34
X52.525 Z-3.518 C-130.785 F363.47
X52.5 Z-3.407 C-130.808 F381.33
Z-2.912 C-130.913 F383.63
Z-2.803 C-130.957 F675.88
Z-2.703 C-131.039 F1189.48
Z-2.616 C-131.155 F1662.46
Z-2.548 C-131.3 F2145.36
Z-2.501 C-131.467 F2693.41
Z-2.478 C-131.646 F3395.33
Z-2.479 C-131.829 F4262.68
Z-2.585 C-133.165 F3714.75

so my C is rotating now.. any how i wanna thank you all for your help ! 

[Anonymous]

here is the code, 
i try to addept this to my working piece and i cant get it to work. @Anonymous would you feel comfirtable to help out on discord or teamviewer ?
I get things way better when i see it or if i cant talk to some one. I understand what i did wrong. I`m really well know with Solidworks and Solidcam but i had to switch software and im just +-3 days in this software. 

Thanks every one for your help. 

[Anonymous]

---

@Anonymous wrote:

here is the code, 
i try to addept this to my working piece and i cant get it to work. @Anonymous would you feel comfirtable to help out on discord or teamviewer ?
I get things way better when i see it or if i cant talk to some one. I understand what i did wrong. I`m really well know with Solidworks and Solidcam but i had to switch software and im just +-3 days in this software. 

Thanks every one for your help. 

---

I am very much self thought in what covers my needs and beyond but I don't consider myself qualified to teach any subject past area of my domain.

Fusion is not that complicated to learn, if you have background in similar software just poke with options and build on small discoveries, it adds up over time.