Have a question or comment about CAM? This is where discussions and questions around CAM and G-code are discussed.
- Various CAM options
- Learning CAM for 5-axis CNC
- Issues or questions on G-code
- What posts are developed for the Pocket NC
brand new here, been a machining for about 5 years in fusion just now getting into more than 3 axis stuff. I have found that the support for this kinda stuff is amazing so far. purchased a used v2-10 about a month ago and have been able to get some very basic cuts on it. wanting to push it a bit more and learn. currently learning 5 axis is a hobby for me, so I cant put as much effort into it as i would like to. currently having a issue with posting anything that is more that indexing tool paths its goes though a tool measuring cycle and before it finishes up i get a alert saying there is unknown gcode being used. I do not have the kinetic control yet, would anyone be willing to help me troubleshoot this at all ?
You’ll need Kinetic Control if you want to use TCPC, which is required to use work offsets with continuous 5-axis tool paths. Otherwise, you’ll need to program your tool paths around the center of rotation of the machine and make sure the use TCPC checkbox is unchecked in your post processor option.
I can see that John from our software development department has responded. I would make sure that you do not have TCPC enabled in your CAM’s post processor. The Pocket NC’s older user interface does not support TCPC (codes M428 and M429) and it is likely the cause of the unknown g-code. You can perform 5-axis machining with your Pocket NC and the older “Legacy” user interface but you will have to program your tool paths around the machine’s center of rotation. I have attached the “Legacy” version of the Pocket NC manual. Click here to access our Legacy V2 Series Work Coordinate System Tutorial.
If you are just performing 3+2 (or indexed) tool operations, then visit our Rotated Work Offsets Tutorial, click here.
If you have any more questions, reach out to us via service@pocketnc.com.
oh cool ill look into that in my gcode, thanks
ill check that out, thank you . getting the kinetic controller is next on my list of things to get, but i gotta recover financially from purchasing the machine first.
looked into it. i did see a M428 in it. i was able to delete that from the program but to the same result. im assuming there is a setting i can change in my setup inside fusion that would get rid of the need to go through and manually delete the line of code ?
Thanks again
There’s a Use TCPC checkbox in the Post Processor window that needs to be unchecked.
Since there is an M428 in your program, there will be a corresponding M429 command, which disables TCPC. You might have Rotary Unwind (M999) selected. This will also need to be disabled.
If you are using Fusion, then you will want to uncheck Use TCPC mode and Use M999 in the post-processor settings (see below).
from what i recall they were both unchecked when i posted this last one, ill run it again when i get to my lunch break. I actually think it was John that helped me with that one on FB a few days ago. if it would help I can post the Gcode here ?
Thanks again
Send me your program and I’ll take a look at it.
since im a new user it doesnt want me to share anything. Should i email it to you?
I made you a regular user, so you should be able to attach G code programs to a post now.
I’m taking a look at your program right now. I’ve loaded it into our simulator, which is available from our website. The simulator is not indicating any issues.
Out of curiosity, what version of the user interface software are you using. Navigate to the Conf. tab, select Version, and then scroll down the Software window until you see a highlighted version (see image below).
The last update to the Legacy Software is version 4.8.1. Let me know if your software version is lower than this release and I will send you a link to version 4.8.1. I will also need your machine’s serial number (click here to discover your machine’s serial number) since the software update process overwrites the machine’s calibration data.
The code G6.2 is also not supported in legacy and is used as part of TCPC. The best solution is to uncheck the use TCPC checkbox so those aren’t used.
serial number on my machine is 1415, the software version thats highlighted is v4.8.1. ill post the raw gcode here and a screen snip of my post screen.
Thanks again guys
1001.ngc (30.3 KB)
Thank you for the screenshots.
Our team has spotted the issue.
The “Use machine configuration” checkbox needs to be unchecked (see below). Checking this box ignores the Post Properties settings (and basically enables TCPC and Use M999). Once this is accomplished, repost your program.
Examining the code that you sent us, we can see that there are codes left in the file that are used for disabling TCPC (see below).
Let us know if this resolved your issue. Thanks for being patient.
Cool I’ll check into that when I get back to work. I’m out for a while though had a family emergency I have to deal with.
Thanks again
Swung by the shop tonight to test it, ran without stock and it did what I expected it to ! Thank you so much guys!