Not profiling corner , rounding corner off instead
-
- Vectric Apprentice
- Posts: 70
- Joined: Wed Aug 29, 2012 4:10 am
- Model of CNC Machine: blackfoot4x8
Not profiling corner , rounding corner off instead
Toolpath rectangle view shows nice angular corner. But when on cnc table the machine is making a large rounded off corner instead of the sharp corner as per preview.
Also the toolpath start point at upper left hand corner in pic does not meet the end point ,slight gap. how do we reset start point, and have the cutter go past the start point ensuring that the whole vector is cut accordingly?
Am now using vcarve pro 8.Still new with this version.
Note am using a 90 degree vbit profiling down to 0.25" and on the vector.
Will try to post the crv file next.
Appreciate any assistance.
A
Also the toolpath start point at upper left hand corner in pic does not meet the end point ,slight gap. how do we reset start point, and have the cutter go past the start point ensuring that the whole vector is cut accordingly?
Am now using vcarve pro 8.Still new with this version.
Note am using a 90 degree vbit profiling down to 0.25" and on the vector.
Will try to post the crv file next.
Appreciate any assistance.
A
- Ms Wolffie
- Vectric Wizard
- Posts: 2695
- Joined: Sat Mar 31, 2012 10:41 pm
- Model of CNC Machine: Blue Elephant 1325, Shark HD Pro
- Location: Tully Heads, Wet Tropics, Queensland, Australia
Re: Not profiling corner , rounding corner off instead
Looks like you have an open vector. Click on it, then click on"close vectors to a common point"lagadishimorto wrote: Also the toolpath start point at upper left hand corner in pic does not meet the end point ,slight gap. how do we reset start point, and have the cutter go past the start point ensuring that the whole vector is cut accordingly?
Appreciate any assistance.
A
That ought to fix that issue
Cheers
Wolffie
Whatshammacallit
Cut3D, VCarvePro 6.5, Aspire4, PhotoVCarve, Corel Graphics Suite X6
Wolffie
Whatshammacallit
Cut3D, VCarvePro 6.5, Aspire4, PhotoVCarve, Corel Graphics Suite X6
- TReischl
- Vectric Wizard
- Posts: 4643
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: Not profiling corner , rounding corner off instead
Need to adjust your machine parameters. Those type of rounded corners are typical of a machine not being set up correctly.
"If you see a good fight, get in it." Dr. Vernon Johns
-
- Posts: 26
- Joined: Fri Jul 06, 2012 5:23 am
- Model of CNC Machine: CamMaster Stinger II SR44
- Location: Arizona, USA
Re: Not profiling corner , rounding corner off instead
In addition to fixing the vectors you should also be aware that any rotating tool cannot produce both inside and outside sharp corners at the same time with a Profile Toolpath strategy. What you need to do is have a closed vector and offset it outward a small amount. Then select both vectors and use a V-Carve Toolpath strategy with a V-bit
C. Andries AKA sscooter
Aspire 11 Laser Module
SR44 Servos, 1.7Kw Spindle, Phenolic Top, WinCnC
Aspire 11 Laser Module
SR44 Servos, 1.7Kw Spindle, Phenolic Top, WinCnC
-
- Vectric Wizard
- Posts: 586
- Joined: Sat Jan 08, 2011 12:29 pm
- Model of CNC Machine: Professional done home built.
- Location: SW Michigan
Re: Not profiling corner , rounding corner off instead
a bug is a flaw that causes a software failure.
This would be more like an unwanted result. Thus not a bug.
This would be more like an unwanted result. Thus not a bug.
- martin54
- Vectric Archimage
- Posts: 7348
- Joined: Fri Nov 09, 2012 2:12 pm
- Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
- Location: Kirkcaldy, Scotland
Re: Not profiling corner , rounding corner off instead
What control software are you running, I've read posts on the mach3 forum where people have had problems like that because of the way the machine had been set up. Is this a new problem since upgrading & did this particular file cut the way you wanted previously.
-
- Vectric Wizard
- Posts: 1715
- Joined: Sun Sep 23, 2012 12:14 pm
- Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"
Re: Not profiling corner , rounding corner off instead
It's the G64 G-code that is causing your problem. Open your post processor with a text editor and look for any instance where G64 is used. It is likely G64 with nothing after it, or G64P.1 or some number after the P.
G64 with nothing after it tells the CNC to run at best possible speed, which may include short-cutting (rounding) corners. Change it to G4P.01 or G64P.001 and it will keep within .01 or .001 of your vector end points. To remove a little of the choppiness use a larger number, but realize that with a larger number it will round the corners more.
http://linuxcnc.org/docs/html/gcode/gcode.html#sec:G64
G64 with nothing after it tells the CNC to run at best possible speed, which may include short-cutting (rounding) corners. Change it to G4P.01 or G64P.001 and it will keep within .01 or .001 of your vector end points. To remove a little of the choppiness use a larger number, but realize that with a larger number it will round the corners more.
http://linuxcnc.org/docs/html/gcode/gcode.html#sec:G64
-
- Vectric Apprentice
- Posts: 70
- Joined: Wed Aug 29, 2012 4:10 am
- Model of CNC Machine: blackfoot4x8
Re: Not profiling corner , rounding corner off instead
Machine post processor is Mach3 .
"Need to adjust your machine parameters. Those type of rounded corners are typical of a machine not being set up correctly."
What machine parameters in Mach 3 do we need to adjust?
"Need to adjust your machine parameters. Those type of rounded corners are typical of a machine not being set up correctly."
What machine parameters in Mach 3 do we need to adjust?
-
- Vectric Wizard
- Posts: 1129
- Joined: Thu Jul 18, 2013 4:58 pm
- Model of CNC Machine: homebuild / VCP 8.0
Re: Not profiling corner , rounding corner off instead
You can do a search on the Mach3 forum for "corner rounding" or even a search on this forum will yield info.
http://www.machsupport.com/wp-content/u ... ngs_v2.pdf
http://www.machsupport.com/wp-content/u ... ngs_v2.pdf
- TReischl
- Vectric Wizard
- Posts: 4643
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: Not profiling corner , rounding corner off instead
4D:
I did a search of the Mach 3 manual, I could find nothing about setting a P parameter with G64. Would you happen to have some info on that in regards to Mach 3?
I did a search of the Mach 3 manual, I could find nothing about setting a P parameter with G64. Would you happen to have some info on that in regards to Mach 3?
"If you see a good fight, get in it." Dr. Vernon Johns
- dealguy11
- Vectric Wizard
- Posts: 2486
- Joined: Tue Sep 22, 2009 9:52 pm
- Model of CNC Machine: Anderson Selexx 510
- Location: Henryville, PA
Re: Not profiling corner , rounding corner off instead
It's been a long time since I used Mach 3, but the settings that control this behavior are are the General Configuration screen. There is one on the right side of the screen that allows you to turn off CV (continuous velocity, if I remember right) when the angle is greater than some value. Setting it in the vicinity of 90 degrees +- 5 degrees should stop this behavior.
Steve Godding
Not all who wander (or wonder) are lost
Not all who wander (or wonder) are lost
-
- Vectric Wizard
- Posts: 1715
- Joined: Sun Sep 23, 2012 12:14 pm
- Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"
Re: Not profiling corner , rounding corner off instead
I don't use Mach2/3/or 4 so I can't give any specific info about those. I did take a quick look at the Mach2/3 post processors for VCarve 7.5 and notice the G64 command isn't used in them. That means it is up to your control software to send it to the CNC. If there is an initialization file that is sent every time your CNC is started up then G64P0.01 could be added to that. If you can type in and send G-code commands to the CNC within the Mach3 window then you could simply send G64P0.01 (or G64P0.001) right before running your file. The machine should remember this code as long as it is powered on, and may even remember it until another G64 or G61 code cancels it out.TReischl wrote:4D:
I did a search of the Mach 3 manual, I could find nothing about setting a P parameter with G64. Would you happen to have some info on that in regards to Mach 3?
- TReischl
- Vectric Wizard
- Posts: 4643
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: Not profiling corner , rounding corner off instead
Constant velocity can be turned on/off and adjusted within Mach3. As far as "including" it in the program? That can be done easily in the post processor, just put it in one of the startup lines and it will always be there.4DThinker wrote:I don't use Mach2/3/or 4 so I can't give any specific info about those. I did take a quick look at the Mach2/3 post processors for VCarve 7.5 and notice the G64 command isn't used in them. That means it is up to your control software to send it to the CNC. If there is an initialization file that is sent every time your CNC is started up then G64P0.01 could be added to that. If you can type in and send G-code commands to the CNC within the Mach3 window then you could simply send G64P0.01 (or G64P0.001) right before running your file. The machine should remember this code as long as it is powered on, and may even remember it until another G64 or G61 code cancels it out.TReischl wrote:4D:
I did a search of the Mach 3 manual, I could find nothing about setting a P parameter with G64. Would you happen to have some info on that in regards to Mach 3?
I don't believe that Mach 3 will use the "P" parameter you wrote about since nowhere in the docs does it mention anything about a "P" parameter in conjunction with G64.
Soooo, for someone like me, I have CV turned on in Mach and set up the way I like it to run. I have no need to turn it on via gcode. If I needed to turn it off for some reason I could just put in a G61. Frankly, in over 35 years of dealing with CNC machines I have never turned CV off. Doing that has a nasty tendency to produce overcuts as the tool pressure is relieved when the machines grinds to a halt in a corner.
BTW, I typically run my machine at 150 - 200 IPM feedrate. Going around a rectangle does not produce any noticeable rounding of the corners. IIRC, Mach 3 adjusts the CV via angles rather than distances. I am too lazy to look it up today. . . . .
"If you see a good fight, get in it." Dr. Vernon Johns
-
- Vectric Apprentice
- Posts: 70
- Joined: Wed Aug 29, 2012 4:10 am
- Model of CNC Machine: blackfoot4x8
Re: Not profiling corner , rounding corner off instead
We've attached the cut file for those who are GCode literate. We don't see mention ofG64 in the TXT.
Again using Mach 3 Arcs inch txt processor.
Thanks
A
Again using Mach 3 Arcs inch txt processor.
Thanks
A
- Attachments
-
- Profile INSIDE BORDERS.txt
- GCODE txt Mach 3 post processor
- (3.9 KiB) Downloaded 236 times
-
- Vectric Apprentice
- Posts: 70
- Joined: Wed Aug 29, 2012 4:10 am
- Model of CNC Machine: blackfoot4x8
Re: Not profiling corner , rounding corner off instead
we just ran another rectangle and noticed the following.
Running Vbit 90 degrees at 13000 rpm at 210 ipm cut to 0.0625 inch deep. When I slowed the federate down as vbit was approaching the 90 corner it made a mauch sharpe corner than when I didn't slow it down for the other corners. So we believe the speed has lots to do with it making a sharper corner. the vcarve preview is consistent in showing sharp corner.Still have not been able to find what setting in MACH 3 tales care of this issue.
Running Vbit 90 degrees at 13000 rpm at 210 ipm cut to 0.0625 inch deep. When I slowed the federate down as vbit was approaching the 90 corner it made a mauch sharpe corner than when I didn't slow it down for the other corners. So we believe the speed has lots to do with it making a sharper corner. the vcarve preview is consistent in showing sharp corner.Still have not been able to find what setting in MACH 3 tales care of this issue.