Hello Guest it is October 15, 2021, 07:28:19 PM

Author Topic: LazyCam, post and other questions  (Read 14132 times)

0 Members and 1 Guest are viewing this topic.

LazyCam, post and other questions
« on: April 07, 2008, 04:26:42 PM »
I finally found out how to post (the "new" post button is real small on my monitor)
I did post questions re Lcam on the Yahoo group and normally a responce is real quick but it
seems the guys over there are very busy discussing Acceleration, newtons, g forces
and the relative merits of same in 3D milling.

That post went as follows:

Is there a way to cancel the default post processor? I don't need the
G91.1, M9, G41 H3. I'm growing tired of editing those items out.

Also Lcam likes to insert a move to safe height at the end of each
pass through a multipath depth cut, why? again I am growing tired of
editing out this move.

Is there any further development happening with Lcam. I find a number
of irritating foibles with it which I know could be corrected and
make the Lcam even better than it already is.

I find that there are too many different places and screens that must
be visited so as to complete all of the information required to get a
good tool path. It's just too easy to make a mistake or forget to
enter all the info.

I'm no expert in CNC machinging but I worked in other areas where
human input is required, parameter inputs were always kept in one
place and usually kept in a logical sequence. Why is it still
required to enter a tool diameter in the offset screen and yet still
have to separately enter a tool in the tool window, would this not
normally be the same diameter as that use in the offset window?
Perhaps this is something to do with the use of offsets setup by appropriate G codes
 (Instructions in a manual would likely help here).

Has any one compiled a basic listing of how to setup Lcam? How does
one set up a personal safe height that Lcam defaults to rather than have
to accept the 1.0000 it now insists on presenting, is there a place
to change this?

How does one write ones own post processor, what is the format of a
post processor? Is it proprietry?

I bought a pro license sometime ago, the outlook for Lcam looked
pretty good then but progress appears to have stalled. I've had license for Mach for over three years .

I'm just hoping I will be able to navigate back to this thread to pickup any answers.
I'd much rather be unravelling some brass than wrestling with the labarynth of links
required to get around the internet to get answers. Once again a manual (hint hint) would be real peachy.

Mike


Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: LazyCam, post and other questions
« Reply #1 on: April 08, 2008, 01:42:04 PM »
Afraid I dont use LazyCAM so  I cant be of much help, however you may have more luck with this in the LazyCAM part of the forum so I will move it there for you.

Hood

Offline Chip

*
  • *
  •  2,055 2,055
  • Gainesville Florida USA
    • View Profile
Re: LazyCam, post and other questions
« Reply #2 on: April 08, 2008, 05:44:10 PM »
Hi, Mike

LC is still under development and needing further work for sure, Mach3 has side-tracked work on it allot.

Saving your work in, File, "Save  LCam project as" should save your settings for that file.

In your C:\Mach3 folder you'll will find a Sub-Dir called "LCamSamples", It has what your looking for on Post's.

Hope this Helps, Chip
Re: LazyCam, post and other questions
« Reply #3 on: April 10, 2008, 10:40:01 AM »
Thanks for replies and getting me shifted over to this part of the Mach forum. I'm having some difficulty navigating back here and being able to post further queries. Any, way the Lcam Samples directory does not address any of the questions I posed. The subdirectory contains a number of DXF, PLT, HPGL and HPG files, nothing to do with PST files. I am still left without an answer as to how to inhibit the default post processing that Lcam insists on doing as it post it's code. Also the process of saving a file in order to preserve any settings is all very well but I generate many new files and it would be real convenient to have a set of default parameters that are mine and not those of some "best guess" by a hard wired program. I'm sure there must be some way to do this already built into Lcam.

Mike

Offline Chip

*
  • *
  •  2,055 2,055
  • Gainesville Florida USA
    • View Profile
Re: LazyCam, post and other questions
« Reply #4 on: April 10, 2008, 05:01:24 PM »
Hi, Mike

What ver. of Mach3 are you using, Help About will tell you.

Maybe thy were files I added to the sub-Dir, Hear thy are below.

Thanks, Chip
Re: LazyCam, post and other questions
« Reply #5 on: April 10, 2008, 05:14:40 PM »
Thanks, I just downloaded the doc.zip. Give me a chance to read and wait for a million more questions, I just know there is a pony in there somewhere

Mike
Re: LazyCam, post and other questions
« Reply #6 on: April 10, 2008, 06:38:57 PM »
Sorry, I forgot to mention that I am running v3.038 of Mach3.  Had a quick look at the zip file. I will have some questions but in the meantime I searched my system for any *.pst files associated with Mach or Lcam, could not locate any! Does that mean Lcam is not using any post processing? or is there a set of defaults that are introducing the G43 and G91.1 etc? I don't quite follow the make up of a pst file, it seems like a very cumbersome way to pass setup parameters to a a program but that doesn't mean to say I think it should be done differently  just that I can't quite figure out the format.  i.e.  G(mode), how does that get translated and what does it actually produce in the Gcode listing? Does the postprocessor require all the asterisks to space sections out?

Mike

Offline Chip

*
  • *
  •  2,055 2,055
  • Gainesville Florida USA
    • View Profile
Re: LazyCam, post and other questions
« Reply #7 on: April 10, 2008, 07:48:20 PM »
Hi, Mike

LazyCam has a "Default" Post built into it, Use "Set Post Processor" in Setup menu, Find and load it "Mill Example.PSt"

Hears what I did, Put in ;##--------------------------- note's to show what was being used and how it was being posted.


*******************************ProgramStart**********************************

;1---------------(Program posted with TestPost.pst)


********************************ToolChange***********************************

M5 M9 ;2----------'Turn the spindle and coolant off
M6 T ;3---------------{TOOLNUM} (TOOLChange) 'toolchange and put a note in the code that it is a ToolChange
G43 H ;4----------{TOOLNUM} 'Put in the Tool length offset and it is the same number as the ToolNUm


********************************ChainStart***********************************


***********************************Rapid*************************************

[ G{MODE} ][ Z{RAPIDHEIGHT}]  ;5-------------------(This is a rapid)'This will pick the Z up to the rapidheight
'and with the []'s if the data in the []'s has not changed it will not be put out

'you can have white space :) and a note that is not on a Gcode line

[G{MODE}][ X{XPOS}][ Y{YPOS}] ;6--------'Now move to the X and Y pos that
[{SPINDLEON}] ;7--------- 'Turn on the spindle and if it is on don't put out the M3
[G{MODE}][ Z{ZPOS}] ;8--------'Move down to the height that the move was to end at


***********************************ZRapid************************************
'This is a Z only move to change the hieght of the tool.. this could be changed
'to {RAPIDHEIGHT} but the jobs will take longer to cut
 
[G{MODE}] Z{ZPOS} ;9-------------


************************************Line**************************************

Your G-code will look like this and help you see what's going on.

N5 ;1---------------(Program posted with TestPost.pst)
N10 M5 M9 ;2----------
N15 M6 T1 ;3---------------1 (TOOLChange)
N20 G43 H ;4----------1
N25 ; 4A ChainStart------------
N30  G0   Z1.0000   ;5-------------------(This is a rapid)
N35  X4.3750  Y27.5000  ;6--------
N40 M3 ;7---------
N45  ;8--------
N50 G1  Z-0.5000  F50.00  ;10------------
N55 X4.3750 Y26.8750   F200.00  ;10------------
N60 X4.3750 Y25.6250    ;10------------
N65 X4.1250    ;10------------
N70 X4.1250 Y28.1250    ;10------------
N75 X4.3750    ;10------------
N80 Y27.5000    ;10------------
N85 X4.7500    ;10------------
N90 X4.7500 Y26.8750    ;10------------
N95 X4.7500 Y25.2500    ;10------------
N100 X3.7500    ;10------------
N105 X3.7500 Y28.5000    ;10------------
N110 X4.7500 Y28.5000    ;10------------
N115 X4.7500 Y27.5000    ;10------------


Ver. 3.00.39 has some fixes, But 3.00.40 should be out soon, Nothing to do with LC though.

Thanks, Chip
Re: LazyCam, post and other questions
« Reply #8 on: April 12, 2008, 04:14:52 PM »
Thanks Chip,  Not sure I completely understand.. Am I correct in saying that [Gmode] is a variable containing what was the last G code issued? 
******Chain Start ****** I have never seen come up in the Gcode.
It appears that your note 10 didn't make it in your reply, perhaps it's redundant in as much as the lines where the 10 is appended are appear to be self explanatory. 
If I do not want a particular code in the posted header I guess I simply do not include it in the PST files i.e. just don't put G43 in the Tool Change section? 
I take it that the ******'s are simply separators, seems a cumbersome way to separate out sections but if that's the way it's done who am I to question it.
Are there any more header words like ****tool change***** and ****chain start***?

I do hope that Lcam will be polished up a bit, it's not that far away from real useful. Right now the quirks in it make it more something to play with than to make
stable predictable Gcode.

Mike
Re: LazyCam, post and other questions
« Reply #9 on: April 12, 2008, 05:25:22 PM »
Chip, another qustion. I can't find Mill Example.PSt on my system is that available on ArtSoft site or should it have been in the updates for Mach3?

Mike