BobCAD V28 Centurion 5 post

[EmeraldIsleforg]

I just upgraded to V28 and recently purchased an old Miltronics Partner 1D with a Centurion 5 controller. I downloaded the Centurion 5 post from BobCAD's site & I have a problem with posting a spiral entry. It doesn't output the z move in the arc moves. Does anyone know how to fix this, or if I can get BobCAD to correct it? If I use another post it works fine. Here's an example of what I'm talking about:

T1 M06
S3819 M03
X-1.4293 Y-1.606
G43 H1 Z1. M08
Z0.2
Z0.1
G17 G03 X-1.5731 Y-1.4016 R0.125 F2.
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125
X-1.4293 Y-1.606 R0.125
X-1.5731 Y-1.4016 R0.125

Similar Threads:

• Need Help!- Centurion 64 bit POST
• Need Help!- Centurion IV Post Help.
• MasterCam Centurion 4 post
• bobcad post for centurion 5

[EmeraldIsleforg]

I just downloaded the Centurion 6 SLS miltronics post and it seems to work. The only thing I'm not sure about is if there are other differences that will cause problems later?

[SBC Cycle]

The original post was probably missing the Z variable in the G17 arc move block. It should have the Z feed variable z_f in there somewhere in order to get a helical move:

64. Arc move XY
n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate

[EmeraldIsleforg]

Thanks SBC Cycle! That was the problem.

Since you were able to tell me how to fix that I was able to correct a few other issues that I found with it as well! I'm attaching a copy of the updated post for anyone who might need it. I added G00 to the first rapid move after each tool change, my mill would feed to the feed plane after the second tool change. It now will output a M01 at the end of each tool, before the next tool. It also puts a G32(Z move to tool change position) and G91G28Y0 after that to move the table forward at the end.

The forum didn't like the file extension, so just remove the .txt at the end of the file.

Thanks!

Mike

[SBC Cycle]

Great! Glad it worked for you. I'm positive a future user will appreciate your efforts and thanks for sharing

[EmeraldIsleforg]

Here's an updated POST. I got tapping on my machine working and updated the post for it. Also corrected a couple of other little issues and added a tool list to the top of the program.

[EmeraldIsleforg]

Here's another update. I fixed it so it will add line numbers just at the start of an operation. Also moved the M01 to after the tool change so that the tool gets out of the way, this way you can see the part better. It also adds all the necessary information to Null Tool Change portion so that if you skip over part of it it will turn the spindle on and not crash!
I'm fixing issues with it as I find them, so as always please check your code before running it.