Problem- Assumed Issues with Post

[looped5]

I am running madCAM and generating code for a HASS vmc. I am currently having three issues with the code it produces:

1) ramping into a pocket does not occur despite providing settings in tool path dialog box, the tool simply plunges down the z axis.

2) all circular or arcing paths are coded as several G1 linear paths instead of G2 or G3 arcs, making files unnecessarily large and cut surfaces inaccurate.

3) the Z feed remains the same as X and Y despite differentiation in tool path dialog box. i tried separating the Z from the X and Y in the post text, but this produced erroneous code.

any ideas on how to correct these issues?
post is copied below...

//MadCAM_POST_2003-12-10
*VERSION*
1.0_031210
*FILE_NAME*
Haas
*FILE_EXTENSION*
nc
*FILE_DEST*
c:\postfiles\
*FILTER*
0.005
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*RAPID*
N"lnbr" G0 "x" "y" "z"
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" "x" "y" "z"
*END_SECTION*
*RAPID_RETRACT*
N"lnbr" G0 "x" "y" "z"
*END_SECTION*
*APPROACH*
N"lnbr" G1 "x" "y" "z" F"feed".
*END_SECTION*
*FIRST_CUT*
N"lnbr" "x" "y" "z" F"feed".
*END_SECTION*
*CUT*
N"lnbr" "x" "y" "z"
*END_SECTION*
*TOOL_CHANGE*
N"lnbr" T"toolnr"M6
N"lnbr" S"speed"M3
N"lnbr" G43 H"toolnr"
N"lnbr" M8
*END_SECTION*
*TOOL_STOP*
*END_SECTION*
*PROGRAM_START*
%
O"pgmnr"
N"lnbr" G40G49G80G90
*END_SECTION*
*PROGRAM_END*
N"lnbr" M28 Z0.0
N"lnbr" M28 Y0.0
N"lnbr" M30
%
*END_SECTION*
*LINE_START_NUMBER*
1

[Dan B]

1) What ramp angle are you using? I generally use 2° or 3° and it works for me. I recall there being an issue with very small angles (=< 1°). I'm not sure if that was ever fixed. I think it was, but I can't say for sure (and no time to test right now)

2) Yes you are correct. I believe that's on the agenda to fix in the future.

3) You aren't using the "feedZ" variable on your approach:

*RAPID_APPROACH*
N"lnbr""x""y""z"F"feedz"
*END_SECTION*

and/or

*APPROACH*
N"lnbr"G01"x""y""z"F"feedz"
*END_SECTION*

Hope this helps,

Dan

[looped5]

The ramp angle was 10 degrees, and it was drawn into the tool path. However, it never completely made it into the g-code. It would do a short ramp in some locations, and simply plunge in others.

I tried using "feedz" but then the x and y feeds get overridden by that. Is there a way to do them separately? As I mentioned in my initial post, I split them as follows:

*FIRST_CUT*
N"lnbr" "x" "y" F"feed".
N"lnbr" "z" F"feedz".
*END_SECTION*

This led to all sorts of different anomalies in the code however.

[Dan B]

That's strange. Using the feedZ works for me. I'll attach a screenshot to show the code. In this example I used a vertical plunge just so it would be easy to see the separation (a ramp will combine the Z move so it obscures the point).

As for the ramp angle, 10° does work for me, and by examining the code, it looks good. I see the X and Z moves which create the ramp. I suppose I could trig it out to see if it's actually 10° but I don't think it really matters that much since the point of your original post is that sometimes it plunges.

Here is a copy of my Fadal post. Maybe you can see something here which will help.

//MadCAM_POST_2010-04-02
*VERSION*
1.04
*FILE_NAME*
AV-Fadal
*FILE_EXTENSION*
cnc
*FILE_DEST*
c:\cnc-code\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*END_SECTION*
*FIRST_MOVE*
N"lnbr"G01"x""y"F7500
N"lnbr""coolant_on"
*END_SECTION*
*RAPID*
N"lnbr"G01"x""y""z"F7500
*END_SECTION*
*RAPID_APPROACH*
N"lnbr""x""y""z"F"feedz"
*END_SECTION*
*RAPID_RETRACT*
N"lnbr"G01"x""y""z"F7500
*END_SECTION*
*RAPID_FEED*
7500
*END_SECTION*
*TOOLCHANGE_TIME*
.33
*END_SECTION*
*APPROACH*
N"lnbr"G01"x""y""z"F"feedz"
*END_SECTION*
*FIRST_CUT*
N"lnbr""x""y""z"F"feed"
*END_SECTION*
*CUT*
N"lnbr""x""y""z"
*END_SECTION*
*TOOL_CHANGE*
N"lnbr" (---------------------Tool change happening here. The new tool is:------------------------------)
N"lnbr" (-------------------------"toolname"------------------------------------)
N"lnbr"M6T"toolnr"M3
N"lnbr"H"toolnr"S"speed""zhome"
*END_SECTION*
*TOOLPATH_CHANGE*
N"lnbr"(-------------------------------------------toolpath change with-----------------------------------------)
N"lnbr"(-----------------------------------------------the same tool-----------------------------------------------)
N"lnbr"(------------------------------------------------------T"toolnr"-------------------------------------------------------)
*END_SECTION*
*TOOL_STOP*
N"lnbr"M5
N"lnbr""coolant_off"
*END_SECTION*
*PROGRAM_START*
%
N"lnbr"(Confirm path: This is path #"pgmnr")
N"lnbr"G17G40G80G90
*END_SECTION*
*PROGRAM_END*
N"lnbr"G90G0H0Z0
N"lnbr"M30
%
*END_SECTION*
*LINE_START_NUMBER*
1
*END_SECTION*
*COOLANT_ON*
M8
*END_SECTION*
*COOLANT_OFF*
M9
*END_SECTION*

Dan