Fanuc oi-m Model D post help

[Anonymous]

Good day all.

I'm trying to post-process my first project in Fusion 360, but seem to be having a few issues with the generic Fanuc post. Our machine is an Omnitech Selexx Chief 5x12 nested router...manufactured by Anderson America, but has a Fanuc oi-m Model D controller.

The first few issues I see are as follows...

1. The nc program loads the proper tool, then immediately loads another (wrong) tool.

2. The tool call format is wrong. All our tool calls need to be preceded with a "1", which denotes spindle number. Example...tool 4 would generate as "t14", tool 6 as "t16", etc.

3. The height offset needs to follow the same conventions as the tool call. Example...tool call "t16" needs a height offset as "h16". (see #2)

These are the first issues I see. I'm attaching working posts from Cabinet Vision and AlphaCAM for reference, as well as a good .nc filefrom Cabinet Vision and the incorrect file generated from the Fusion 360 generic Fanuc post.

Any help or guidance would be greatly appreciated. Thank you!

[Anonymous]

Here's the other attachments...

[Anonymous]

Found 2 more issue with the code generated with the Generic Fanuc post...

It is using "M03" for the spindle activation, and for this machine it needs to be "M13".

Also, the "M13" needs to come before the speed "S18000", rather than after, or the spindle doesn't activate.

[Laurens-3DTechDraw]

The second tool call, is to pre-load the next tool.That's why there is no M06 behind.

If your machine doesn't allow for pre-loading you can turn it off in the post properties.

[Anonymous]

Thank you Laurens for the info. I found the “pre-load next tool” switch in the beginning of the post. Changing that to “false” fixed the 2-tool issue. I’ve also found that if I re-number the tools as 11, 12, 13 etc, they do work for tool call and offset call.

What I’m still having an issue with…

1. The “spindle off” code is coming in as “M05”, but needs to be “M15”.

2. The “Spindle on CW” code is coming in as “M03”, but needs to be “M13”.

3. The start spindle command and speed are generated in the wrong order. The line reads “S18000 M03”, but needs to read “M13 S18000”. If the “M13” doesn’t come first, the spindle never starts.

[Laurens-3DTechDraw · Accepted solution]

---

@Anonymous wrote:

Thank you Laurens for the info. I found the “pre-load next tool” switch in the beginning of the post. Changing that to “false” fixed the 2-tool issue. I’ve also found that if I re-number the tools as 11, 12, 13 etc, they do work for tool call and offset call.

What I’m still having an issue with…

1. The “spindle off” code is coming in as “M05”, but needs to be “M15”.

2. The “Spindle on CW” code is coming in as “M03”, but needs to be “M13”.

3. The start spindle command and speed are generated in the wrong order. The line reads “S18000 M03”, but needs to read “M13 S18000”. If the “M13” doesn’t come first, the spindle never starts.

---

Alright.

 This line: 

 writeBlock(
      sOutput.format(tool.spindleRPM), mFormat.format(tool.clockwise ? 3 : 4)
    );

needs to become

 writeBlock(
      mFormat.format(tool.clockwise ? 13 : 14), sOutput.format(tool.spindleRPM)
    );

Also change these lines:

  COMMAND_SPINDLE_CLOCKWISE:3,
  COMMAND_SPINDLE_COUNTERCLOCKWISE:4,
  COMMAND_STOP_SPINDLE:5,

to

  COMMAND_SPINDLE_CLOCKWISE:13,
  COMMAND_SPINDLE_COUNTERCLOCKWISE:14,
  COMMAND_STOP_SPINDLE:15,

[Anonymous]

Worked like a champ! Thank you so much for your time and knowledge...much appreciated! Have a great day! 🙂

[Laurens-3DTechDraw]

Glad you got it working.

[Anonymous]

Hello!

Thank you for posting and getting this thread started after reading through everything has been a big help thus far. I noticed you said that you were able to change tools go from T11,12,13 etc. I couldn't find that part of the code to modify and was wondering if you could point me in the right direction.

Thanks!

[Laurens-3DTechDraw]

---

@Anonymous wrote:

Hello!

Thank you for posting and getting this thread started after reading through everything has been a big help thus far. I noticed you said that you were able to change tools go from T11,12,13 etc. I couldn't find that part of the code to modify and was wondering if you could point me in the right direction.

Thanks!

---

No that part has nothing to do with it.

He just changed the tools in the CAM to T11 instead of T1.

That is the easiest way.

[woodshopcg]

I figuered out the T11,12 but how did you change the post to output the hight compensation H11,12?

[Laurens-3DTechDraw]

Also in CAM.

In the Tool library.

[woodshopcg]

Post seems to work good for my Omnitech sellex Pal  2 things I would like to modify. 

how would I modify the post footer to park the machine at a certain postion

turn off vaccume clamp (M07) at the end of the cycle