Too many g-code lines

This forum is for general discussion regarding VCarve Pro

Too many g-code lines

Postby icncsigns » Tue Jun 17, 2008 7:00 pm

Hello
I use Mach3 & VCP.4.6 I am having a problem with too much g-code produced. An example, cutting out a 8.0" circle 537 lines to make a complete circle I have to stop the router because it will continue to cut the same circle & it drops down the thickness of what was set in the begining
of the job each rotation of the router. The file turns out to have 5300 line of g-code. The job was made in VCP. Help!! what am I doing wrong??? :?
icncsigns
 
Posts: 35
Joined: Tue Jun 17, 2008 6:23 pm

Postby Phil » Tue Jun 17, 2008 7:33 pm

How did you cerate the circle? Did you convert a bitmage to a vector or did you draw the circle with VCarve's drawing tools?
User avatar
Phil
Vectric Wizard
 
Posts: 1760
Joined: Thu Nov 17, 2005 10:56 pm
Location: Pittsfield, MA

Postby icncsigns » Tue Jun 17, 2008 8:47 pm

Thank you for replying
I used v-carve pro. Also it will do the samething when exported from another program into .crv format then into a .tap Then load g-code into Mach. I makes the same excessive code in every file. I loaded vcp into another computer & the outcome was the same. Too much code when loaded into Mach
icncsigns
 
Posts: 35
Joined: Tue Jun 17, 2008 6:23 pm

Postby Phil » Tue Jun 17, 2008 10:19 pm

I's often necessary and helpful to do some editing on the vector file. For example, if the drawing has a circle select it and click the letter "N" for node editing. I'm guessing you will see many black square dots. If you erase that circle and redraw it with the circle drawing tool the circle will only have four nodes. This type of editing will greatly reduce the size of the cut file. Also you will get a much cleaner cut.
User avatar
Phil
Vectric Wizard
 
Posts: 1760
Joined: Thu Nov 17, 2005 10:56 pm
Location: Pittsfield, MA

Postby icncsigns » Tue Jun 17, 2008 11:56 pm

I used v-carves circle drawing tool to make it. I will attach the files.
Thank you for your help.
Attachments
5.5 inside.crv
(217.5 KiB) Downloaded 112 times
icncsigns
 
Posts: 35
Joined: Tue Jun 17, 2008 6:23 pm

Postby icncsigns » Wed Jun 18, 2008 12:00 am

Here is the outside File
Attachments
8.0 outside.crv
(121.5 KiB) Downloaded 77 times
icncsigns
 
Posts: 35
Joined: Tue Jun 17, 2008 6:23 pm

Postby RoutnAbout » Wed Jun 18, 2008 1:53 am

I've downloaded both files.
Both files only have 2 circles.
  • outside circle is 8.0 inches
  • inside circle is 5.5 inches
Both circles are a good clean circle with only 4 nodes each.
I also noticed your material is .063 inches thick.
Your depth per pass is only .0129 inches
.063 inches divided by .0129 inches means your going to have 5 circular passes. (for both large and small circle)
I also noticed that your feed rate is 200 per minute , I don't know if I'd run that feed with that small bit.
I didn't change any of the cam settings and generated the following code for the 8.0 inch circle, consisting of only 41 lines.

Code: Select all
( 8.0 outside )
( Mach2/3 Postprocessor )
N20G00G20G17G20G90G40G49G80
N30G70
N40T1M06
N50G00G43Z0.7874H1
N60S18000M03
N70G94
N80X0.0000Y0.0000F200.0
N90G00X0.6631Y4.4278Z0.2362
N100G01Z-0.0130F20.0
N110G2X4.7568Y8.5216I4.0938J0.0000F200.0
N120G2X8.8506Y4.4278I0.0000J-4.0938
N130G2X4.7568Y0.3341I-4.0938J0.0000
N140G2X0.6631Y4.4278I0.0000J4.0938
N150G01Z-0.0260F20.0
N160G2X4.7568Y8.5216I4.0938J0.0000F200.0
N170G2X8.8506Y4.4278I0.0000J-4.0938
N180G2X4.7568Y0.3341I-4.0938J0.0000
N190G2X0.6631Y4.4278I0.0000J4.0938
N200G01Z-0.0390F20.0
N210G2X4.7568Y8.5216I4.0938J0.0000F200.0
N220G2X8.8506Y4.4278I0.0000J-4.0938
N230G2X4.7568Y0.3341I-4.0938J0.0000
N240G2X0.6631Y4.4278I0.0000J4.0938
N250G01Z-0.0520F20.0
N260G2X4.7568Y8.5216I4.0938J0.0000F200.0
N270G2X8.8506Y4.4278I0.0000J-4.0938
N280G2X4.7568Y0.3341I-4.0938J0.0000
N290G2X0.6631Y4.4278I0.0000J4.0938
N300G01Z-0.0650F20.0
N310G2X4.7568Y8.5216I4.0938J0.0000F200.0
N320G2X8.8506Y4.4278I0.0000J-4.0938
N330G2X4.7568Y0.3341I-4.0938J0.0000
N340G2X0.6631Y4.4278I0.0000J4.0938
N350G00Z0.2362
N360G00Z0.7874
N370G00X0.0000Y0.0000
N380M09
N390M30
%


The code looks good to me.
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2062
Joined: Mon Sep 19, 2005 11:09 pm
Location: North Manchester, Indiana
Model of CNC Machine: Old Bot with a Rope Pull Start Spindle

Postby Mark » Wed Jun 18, 2008 9:32 am

Hello icncsigns,

Try using the "Mach2/3 ATC Arcs (inch)(*.txt)" post processor.
This will greatly reduce the number of lines of G-Code in the file.

Make sure that Your "IJ Mode" within Mach3 is set to "Inc"
(Menu > Config > General Config).

I hope that this helps,

Mark.
User avatar
Mark
Vectric Staff
 
Posts: 910
Joined: Sat Aug 18, 2007 2:55 pm
Location: Redditch U.K.
Model of CNC Machine: None Yet

Postby icncsigns » Wed Jun 18, 2008 2:53 pm

Thank you Don & Mark I will let you know if that fixed it. :)
icncsigns
 
Posts: 35
Joined: Tue Jun 17, 2008 6:23 pm

to much g code

Postby moto633 » Sun Jul 13, 2008 3:22 pm

I am having the same problem with there being to much Gcode being posted in the Mach program. I tried to carve a simple small five letter test sign and it estimated 16min. Did you ever solve your problem? If so how?
Any input would be great!
Thanks,
Nick
moto633
Vectric Wizard
 
Posts: 1120
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

Postby Mark » Sun Jul 13, 2008 3:46 pm

Hello Nick,

I think Icncsigns case was different to yours, he was machining some circles drawn within VCarve Pro, the G-Code needed to produce these
can be just a few lines if the cnc controller is capable of interpreting Arc moves.
Your case is different, if you are VCarving letters, these will be 3D moves
and will involve a fair number of G-Code lines to produce the letters.
The length of time needed to machine these would be dependent on the
feeds and speeds that your machine can support.

I hope that this makes sense.

Mark.
User avatar
Mark
Vectric Staff
 
Posts: 910
Joined: Sat Aug 18, 2007 2:55 pm
Location: Redditch U.K.
Model of CNC Machine: None Yet

Postby moto633 » Sun Jul 13, 2008 4:07 pm

Hey Mark,
Thank you for the reply. I watched the router and it just keeps repeating the cut over and over. The letter looks completed and it just keeps going over the same path.
When I downloaded the trial version and ran the Bullshead sign it only took a few min. My test cut is a simalar size and not nearly as complex. All my settings and feeds are the same as when I ran the trial version test.
Any other suggestions? I'm not very computer savvy so bear with me!!!!
Thank you for your time,
Nick
moto633
Vectric Wizard
 
Posts: 1120
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

Postby Mark » Sun Jul 13, 2008 4:09 pm

Hello Nick,

If you would like to send me a copy of your .CRV file, I will check this out for you.

Cheers,

Mark.

support (at) vectric (dot) com.
User avatar
Mark
Vectric Staff
 
Posts: 910
Joined: Sat Aug 18, 2007 2:55 pm
Location: Redditch U.K.
Model of CNC Machine: None Yet

Postby moto633 » Sun Jul 13, 2008 4:41 pm

Mark,
I sent the file that I use to you at the vectric support email. Hope that it helps.
Thanks,
Nick
moto633
Vectric Wizard
 
Posts: 1120
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

Postby Mark » Sun Jul 13, 2008 4:50 pm

Hello Nick,
It is the .CRV file from VCarve pro that I really need.
This will allow me to check out the pass depths that you have set etc.

Hopefully you will have saved this before you exited VCarve Pro.
If you have a copy, please le me know.

Cheers,

Mark.
User avatar
Mark
Vectric Staff
 
Posts: 910
Joined: Sat Aug 18, 2007 2:55 pm
Location: Redditch U.K.
Model of CNC Machine: None Yet

Next

Return to VCarve Pro - General

Who is online

Users browsing this forum: Google [Bot], modoleinad and 5 guests