Community
PowerMill Forum
Welcome to Autodesk’s PowerMill Forums. Share your knowledge, ask questions, and explore popular PowerMill topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

2D turning post processor for powermill 2017

25 REPLIES 25
SOLVED
Reply
Message 1 of 26
Anonymous
10755 Views, 25 Replies

2D turning post processor for powermill 2017

Hi is there a 2D turning post processor for powermill 2017? We have a Mazak 3 axis Lathe that uses the C-AXIS. Can you use the new turn feature to generate say a simple Hex on the front of a job using the C, X, Z axis. Thanks

25 REPLIES 25
Message 2 of 26
iamcdn79
in reply to: Anonymous

Refer to this topic


Intel Core i9 13900KF CPU
128 GB Kingston Beast DDR4 SDRAM
PNY RTX A2000 6GB Video Card
WD 1 TB SSD Hard Drive
Windows 11 Pro

Message 3 of 26
Anonymous
in reply to: iamcdn79

Hi thank you for the link but I'm still having trouble on how to post in just the X Z and C AXIS. is there a setting I need to change on the setting page on the turning strategies? It seems that theres no clear answers or tutorial on basic post processing for the Powermill 2017.

Message 4 of 26
Anonymous
in reply to: Anonymous

If there is no solution for turning strategies, maybe try to use mill strategies. I don't know how would you like to do this, but in any case, i think i could help you. I try to prepare some examples, but it won't be earlier than Monday morning.

 

 

Mateusz

Message 5 of 26
Anonymous
in reply to: Anonymous

Hi thank you yes that will help a lot. Monday is good.

Message 6 of 26
Anonymous
in reply to: Anonymous

I created an experimental Mill/Turn postprocessor, based on Delcam std. Mazak PP. Please test and edit it if necessary.

Message 7 of 26
Anonymous
in reply to: Anonymous

Thank you I will try them tomorrow and let you know how it goes

Message 8 of 26
Anonymous
in reply to: Anonymous

 Its posted the program from your post but it seems to be for the Mazak multi axis. The machine I have is a Mazak Mazatrol 640MT its a CNC lathe 3 axis with just the C axis. Im not to experienced with editing the post processors. For example on the lathe to select a tool you call up T0303 (TOOL 3 OFFSET 3) rather than T3 M6 then later on G43 H3. Is there away to use this post processor but edit it. Ive attached a sample Power mill project I used to test your post processor on. Thanks.

Message 9 of 26
Anonymous
in reply to: Anonymous

Hi!

Tool call changed to T0303 (TOOL 3 OFFSET 3) . All comment line  temporary disabled. The PP is not a real five axis machine, handling only "3AXIS" and   "2AXIS_XZ" Axis Modes.

The five axis kinematic required only for simplify Mill-Turn postprocessing.

Please write a short NC sample for turning and milling so i can adapt it.

Thanks.

Message 10 of 26
Anonymous
in reply to: Anonymous

 Ive tried the program on the machine but it cannot recognise the format  I AND J (eg G2 X15.0 C5.774 I-4.33 J-2.5.) when looking for and example on the internet ive found this format works  G2 X1.8274 C0.5499 R1.075 (using just C and R) I will attach a sample program using the C-AXIS that I found on the internet for you to look at. The machine im on is a Mazak Fusion 640MT. (PS this example in in imperial I run the machine in metric) Thanks

Message 11 of 26
Anonymous
in reply to: Anonymous

I use attached manual. See 6-19 (page 63).

The two arc  definition equal: 02/G03 XY R and G02/G03 XY IJ. If you want i  use "R" format instead "IJ".

 

Message 12 of 26
Anonymous
in reply to: Anonymous

yes will this be the same as the Mazak 250 - II M version or will this be different as I don't have access to any manuals here

Message 13 of 26
Anonymous
in reply to: Anonymous

Here ive attached the sample program that we use for turning could you add the part name, cycle time and tool description to the post thank you. I hope this will solve it.

Message 14 of 26
Anonymous
in reply to: Anonymous

Largely succeed adapt the turn pp. Please test it.

Your machine how to switch:

- diameter/radius mode (G10.9) ?

-milling mode on/off (M200/M202) ? 

- select XC plane (G17XC) ?

- polar coordinate interpolation on/off (G12.1/G13.1) ?

Thx.  

Message 15 of 26
Anonymous
in reply to: Anonymous

 Yes this is working the only issues are the spindle speed clamp (G50 S1000) isn't altering when you change it in the speeds and feeds menu plus the G96 and G97 and there speed values don't change either. Is there away to generate the program in diameter value rather than radius value? And one last thing is that there are three lines after the tool cancel and M1 that are not needed,

Z-7.686 (***THIS LINE IS NOT NEEDED***)
Z2 (***THIS LINE IS NOT NEEDED***)
M1(*** THIS LINE IS NOT NEEDED**)

 

Regarding the other G codes you mentioned

- diameter/radius mode (G10.9)  YES

-milling mode on/off (M200/M202) YES

- select XC plane (G17XC) YES

- polar coordinate interpolation on/off (G12.1/G13.1)  YES

 

I have attached a simple turning project and the program and in brackets you will see the issues highlighted. 

Thank you

Message 16 of 26
Anonymous
in reply to: Anonymous

Some minor improvements:
Turning -Diameter mode ON
Turning+Milling: Joins suppressed.
 
I have a lot of work tomorrow and the day after so I won't be able to help out then, but I will look into it during this weekend.

Message 17 of 26
Anonymous
in reply to: Anonymous

New version, please test it.

The PP get Spindle Clamping Speed from first toolpath Maximum Speed, if Constant Surface Speed is active else set 3000 rpm.
For proper PP operation please set turning Feed Units Per revolution, milling Feed Units set Per minute. (pic 1.)
The PP Diameter mode  adjustable in PP Option File Settings (pic 2.)

 

Feeds.JPG

 

DiameterMode.JPG

 

 

 

Message 18 of 26
Anonymous
in reply to: Anonymous

Thank you for your help Vékási Tibor it works great.

Message 19 of 26
Anonymous
in reply to: Anonymous

hello friend i need post processor fanuc turning formates 

Message 20 of 26
lxc
Enthusiast
in reply to: Anonymous

Hi.

I would like to add two turning allowances to your post processing:Turning.RoughXThickness,Turning.RoughZThickness

How to increase?

Thank you.2019-05-22_09h19_24.png


@Anonymous wrote:

New version, please test it.

The PP get Spindle Clamping Speed from first toolpath Maximum Speed, if Constant Surface Speed is active else set 3000 rpm.
For proper PP operation please set turning Feed Units Per revolution, milling Feed Units set Per minute. (pic 1.)
The PP Diameter mode  adjustable in PP Option File Settings (pic 2.)

 

Feeds.JPG

 

DiameterMode.JPG

 

 

 


 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Technology Administrators