Page 1 of 1

About Post processor: MP1000-THC.scpost

Posted: Wed Jul 03, 2019 8:37 pm
by kessordi

N0020 (Post processor: MP1000-THC.scpost)
N0040 G21 (Units: Metric)
N0050 G53 G90 G40
N0060 F1

N0100 G00 Z0025
N0110 X41.4191 Y23.3284
N0120 Z0025
N0130 G28.1 Z10.00
N0140 G92 Z0.0
N0150 G00 Z0.0000
N0160 G92 Z0.0
N0170 G00 Z6.0000
N0180 M03

can i know haw to change the feedrate for those two lines ( N0130 G28.1 Z10.00 )
(N0140 G92 Z0.0 )

while the torch come down looking for metal it come down slowly


Re: About Post processor: MP1000-THC.scpost

Posted: Thu Jul 04, 2019 9:17 am
by robertspark
what machine are you running this post processor on?
Mach3, Mach4, LinuxCNC?

In Mach3
G28.1 Reference Axis
Program G28.1 X~ Y~ Z~ A~ B~ C~ to reference the given axes. The axes will move at the current feed rate towards the home switch(es), as defined by the Configuration. When the absolute machine coordinate reaches the value given by an axis word then the feed rate is set to that defined by Configure>Config Referencing. Provided the current absolute position is approximately correct, then this will give a soft stop onto the reference switch(es).
G92 does not do any motion, it just sets the axis offset (a temporary offset)
G92,G92.1,G92.2 & G92.3 Offsets
See the chapter on coordinate systems for full details. You are strongly advised not to use this legacy feature on any axis where there is another offset applied.

To make the current point have the coordinates you want (without motion), program
G92 X~ Y~ Z~ A~ B~ C~ , where the axis words contain the axis numbers you want. All axis words are optional, except that at least one must be used. If an axis word is not used for a given axis, the coordinate on that axis of the current point is not changed. It is an error if:

ยจ all axis words are omitted.

G52 and G92 use common internal mechanisms in Mac and may not be used together.

When G92 is executed, the origin of the currently active coordinate system moves. To do this, origin offsets are calculated so that the coordinates of the current point with respect to the moved origin are as specified on the line containing the G92. In addition, parameters 5211 to 5216 are set to the X, Y, Z, A, B, and C-axis offsets. The offset for an axis is the amount the origin must be moved so that the coordinate of the controlled point on the axis has the specified value.

Here is an example. Suppose the current point is at X=4 in the currently specified coordinate system and the current X-axis offset is zero, then G92 X7 sets the X-axis offset to -3, sets parameter 5211 to -3, and causes the X-coordinate of the current point to be 7.

The axis offsets are always used when motion is specified in absolute distance mode using any of the fixture coordinate systems Thus all fixture coordinate systems are affected by G92.

Being in incremental distance mode has no effect on the action of G92.

Non-zero offsets may be already be in effect when the G92 is called. They are in effect discarded before the new value is applied. Mathematically the new value of each offset is A+B, where A is what the offset would be if the old offset were zero, and B is the old offset. For example, after the previous example, the X-value of the current point is 7. If G92 X9 is then programmed, the new X-axis offset is -5, which is calculated by [[7-9] + -3]. Put another way the G92 X9 produces the same offset whatever G92 offset was already in place.

To reset axis offsets to zero, program G92.1 or G92.2 G92.1 sets parameters 5211 to 5216 to zero, whereas G92.2 leaves their current values alone.

To set the axis offset values to the values given in parameters 5211 to 5216, program G92.3

You can set axis offsets in one program and use the same offsets in another program. Program G92 in the first program. This will set parameters 5211 to 5216. Do not use G92.1 in the remainder of the first program. The parameter values will be saved when the first program exits and restored when the second one starts up. Use G92.3 near the beginning of the second program. That will restore the offsets saved in the first program.

Re: About Post processor: MP1000-THC.scpost

Posted: Thu Jul 04, 2019 10:54 am
by djreiswig
I think it's because you have the feedRate set to 1 on line 60. I don't think you are getting a feedrate setting from your tool. What happened to lines 70-90?

Re: About Post processor: MP1000-THC.scpost

Posted: Thu Jul 04, 2019 12:49 pm
by Les Newell
Go to Options->machine->post processor and click the 'Edit post' button.
Starting on around line 100 you should see this code:

Code: Select all

function OnPenDown()
   if(dist >= (refdistance/scale)) then
      dist = 0
--      modaltext (" G00")
--      text(" Z")
--      number (pierceheight  * scale, "0.0000")
--      eol()
      post.ModalText(" G28.1 Z")
      post.Number(3 * scale, "0.00")
Immediately after add this code:

Code: Select all

      post.ModalNumber (" F", 100, "0.0###")
Change the 100 to whatever feed rate you want.

Re: About Post processor: MP1000-THC.scpost

Posted: Sat May 02, 2020 10:34 am
by Steve_hi
Hi I'm having trouble with the same post processor, I am trying to do my first cuts with my home made plasma table I entered the correct height for my cut height 0.06 inch in the tool creation box, but the code generated puts the height at .130 inch I looked at the code code to see if I could edit it but I have no knowledge of programming I'm Just a machinist. I noticed the cutting height is the same as my pierce height. This is my first go at building a CNC machine so sorry if the answer is obvious and I just don't know it.
Thanks for any help.

Re: About Post processor: MP1000-THC.scpost

Posted: Sat May 02, 2020 11:21 am
by Steve_hi
PS im using a floating head with a limit switch

Re: About Post processor: MP1000-THC.scpost

Posted: Mon May 04, 2020 11:43 am
by Les Newell
Set up a job then save it (File->save job). Now run the post processor. If you let me have those two files I'll take a look and see if I can figure out what is going on.