Techno CNC HD post (see attachments)

[cmleschak]

Hey everyone, I am looking to have a post modified to work with our Techno CNC HD model.  The Techno CNC post that is available is for the LC model control which is a little more advanced than the handheld controller we have.  Using HSMExpress for solidworks to make some simple profiles on our router.

I have attached the Techno CNC post I found along with the posted program in text format to show a working and non working.  I am not super familiar with Java Script and while I am working on teaching myself the language, it would be great if someone could help me modify this post to work..

When I ran the program to cut the part the spindle turned on, then I got a G79 not recognized (or something similar) then the spindle shut back off.  I modified the program to match how our old programmers posts used to look coming from VisualMill and it worked great.

I believe that the LC controller uses a G79 to bring Z home before making any other moves. This is not needed on our control.  G40 to shut cutter comp off is not needed because we are comping in the programming software rather than in the control (not even sure this control is capable of calculating cutter comp as there are no tool libraries that I know of)

Our machine also doe not have work offsets (fixture offsets) or a tool changer.

[cmleschak]

Think I figured it out.. Will test at some point this week.  Here is what I came up with by simply turning some of the code on the existing post into effectively notes. 

[cmleschak · Accepted solution]

Last one.. G27 code had to go..

This is a TESTED working post for Techno CNC HD router

Disable HDS setting if you dont have a tool changer and it should work fine!

[agutorov87]

If anyone else stumbles on this post, here is how to get rid of G27:

Tested on the HD Mini, should work for any NC Studio / Weihong controller (Nk105)

The post still shoved a G27 in the code. 

To fix:

• Open the code in Notepad or Notepad++,
• find line398  "writeBlock(gFormat.format(27)); // make sure continuous operation smoothing on"
• insert // at start of line to comment it out.   
• // writeBlock(gFormat.format(27)); // make sure continuous operation smoothing on

Some info:

G27 - Check if point is at zero  - is not recognized, and somewhat outdated.

G28 - move to zero - is recognized 

The G28 command will return to machine zero. (Not the work-piece offset zero)

G28 can be used on its own or with a X# Y# Z#. This will move, at rapid, to the coordinate first, then it will rapid move to zero. 

Example: 

X10 Y10        //tool is at x-10 y-10

G28 X5 Y5    //tool moves to x-5 y-5 , then tool moves to x-0 y-0 

----------------------------------------------------------------------------------------------------------

I will be running through the post processor and seeing what can be changed.

For the HD Mini there are a few issues:

G17-G19 seem to be messing with the rapid moves. I'm not done testing the issue yet, so I'm not sure what the cause is. G00 and G01 should, by default, be G17 (xy-plane) moves. I think the post doesn't add G00/G01, etc on every line of code it is used in. This should be fine, because G00-G03 is modal and will run in that mode until another G code in that group is called. This means that if you use a G00 code, you can do rapid moves with bare coordinates with no prefix until another G0# is used. However, anytime there's bare X# Y# Z# without a prefix, the controller seems to default to the last G/17G18/G19 used. This caused rapids to go to each coordinate in order, and not move in a straight line from point to point.

example:

G18 X# Z# I#  //move in xz plane

G00 X10 Y10  //rapid move, should default to G17

       X20 Y20  //should be rapid move G00, but is not G17 by default. 

This causes:

Rapids to X10,Y10

Rapids to X10 first, then to Y20

It should be:

G00 X10 Y10   //Rapids to X10, Y10

G00 X20 Y20  //Rapids to X20 Y20 in a straight line

I'll try to update this after I run some tests. 

[ben.drexl]

Your post (with the G27 commented out) seems to work great with the Baileigh CNC router table we have here. It uses the NK105 G2 controller.

I ran one fairly basic test, but included some ramps and everything went as expected.

Thanks!