Please help with engraving problem

This forum is for general discussion regarding VCarve Pro

Please help with engraving problem

Postby wingnut2.0 » Fri Sep 26, 2008 2:14 am

Please see attached pics. I am new to Vectric software and experiencing problems with plate production/text engraving. I am not positive the is a Vectric issue, could be a controller (mach3) issue. There appears to be some sort of "ramp" into and out of a few of the letters in the attached pics (see U's L's and H's). I have followed the plate production .pdf so I am assuming this might be a mach3 issue. Looking for some input from those that might have experienced this.

CV is enabled and set for 180.00 (180 what?)

Thanks.
Attachments
HPIM0770.JPG
Example of problem
wingnut2.0
 
Posts: 5
Joined: Thu Sep 25, 2008 3:20 am

Postby Regnar » Fri Sep 26, 2008 2:30 am

I dont use mach3 but I know people over on the zone have had problems using CV mode and most disable it. It tries to keep everything moving at the same seed will round corners so I imagine it will do it to the z axis as well. Again I dont use mach so take my advice with a grain of salt. Hope it helps though.
User avatar
Regnar
Vectric Apprentice
 
Posts: 92
Joined: Fri Apr 20, 2007 2:22 am

Re: Please help with engraving problem

Postby RoutnAbout » Fri Sep 26, 2008 2:46 am

Hello and welcome to the forum Wingnut.
I know very little about Mach3 software, but from the images you've posted.

If you look close at each letter and the profile cut. There is a distinct difference that the tool is entering and exiting your vectors.
I'm guessing this is a single line font.

I'm also assuming that you generated the code to machine ON vectors.
And at the begining or the end of the vector your tool is ramping into or out of your letters.

I think this really has something to do with settings in your control software.
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2056
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 wingnut2.0 » Fri Sep 26, 2008 3:14 am

Regnar & RoutnAbout,

Thanks for getting back so quickly. The toolpath for the single line (Helvetica 1L) is set for ON vector and I have made all the mach3 setting changes recommended on the zone as well as the mach forum. I will keep digging and update this thread with whatever I find. Thanks again.

PS What control software are you using?
wingnut2.0
 
Posts: 5
Joined: Thu Sep 25, 2008 3:20 am

In defense of CV mode in Mach 3

Postby HoustonFirefox » Fri Sep 26, 2008 4:23 pm

About the CV mode confusion in Mach 3:

I've heard several people mentioning that they had problems using it. I know I did awhile back when I tried to pocket squares and the corners at opposite ends kept getting rounded. Here is what I found out;

The CV mode attempts to keep the cutter moving at the last commanded feed rate throughout all movements below the set CV rate (in this case 180). What that means is that if the next move is more than 180 degrees relative (in this example) to the current cutter path then the machine is commanded to full stop (absolute mode) before the next move is made.

The problem arises when there is, say, a 90 degree movement perpendicular to the current path of the cutter. In order to make the 90 degree move, the software will attempt to "round-out" the move in an attempt to keep the feed rate constant. This is not what we want since the corners of a square pocket would be rounded. This happens because (in our example) more than a 180 degree movement has not been commanded, just a motion 90 degrees relative to the last path.

Important: Remember that the CV mode also acts on the Z axis as well.

It would seem, at first glance, that to turn CV mode off would be the best option but I have found that all this does is put the machine in "absolute stop" mode at the end of each line segment (think segmented circle here). This would then cause the machine to ramp up and down on each itty-bitty little line segment, a huge waste of time since the machine spends more time ramping up and down when it really should be moving in a continuous motion.

The solution (or at least it works great for me) is to enable CV mode and change the setting to 45 (degrees; works for me). Now, any movement greater than 45 degrees to the last cutter movement will come to a complete stop, change direction and ramp. Anything less than that will be one smooth motion (Continuous Velocity).

It took me awhile to figure out but my productivity has shot up and the wear on my machine drastically reduced since there are far fewer start-ramp up-go-ramp down-stop cycles of the mass of the gantry. Give it a try on your next project, especially one where you know how long it takes to cut and you'll be amazed at the productivity gains (and smoothness of your machine).

:D
Last edited by HoustonFirefox on Fri Sep 26, 2008 4:55 pm, edited 1 time in total.
CNC Woodworkers do it with a 3D Touch Probe!
User avatar
HoustonFirefox
Vectric Craftsman
 
Posts: 216
Joined: Wed Aug 22, 2007 5:17 pm
Location: Houston, TX

Re: Please help with engraving problem

Postby Rolf » Fri Sep 26, 2008 4:41 pm

wingnut2.0 wrote:Please see attached pics. I am new to Vectric software and experiencing problems with plate production/text engraving. I am not positive the is a Vectric issue, could be a controller (mach3) issue. There appears to be some sort of "ramp" into and out of a few of the letters in the attached pics (see U's L's and H's). I have followed the plate production .pdf so I am assuming this might be a mach3 issue. Looking for some input from those that might have experienced this.

CV is enabled and set for 180.00 (180 what?)

Thanks.


I know this is OFF topic but I noticed that you are using the same margin for both signs. The "PULL" sign has to much white space on the right because of the last "L". This is a common mistake that is made by even old "professionals". On my old engraving machine software I had to use manual kerning until I got he fonts automatic kerning adjusted.
Rolf
 
Posts: 2
Joined: Fri Sep 26, 2008 3:58 pm
Location: E. Tennessee, USA

Help with engraving

Postby Roly » Sat Sep 27, 2008 12:08 am

Houston,
I think I have a problem.

I didn't realise that the cv also affected the Z axis. I finally worked out how it affects the other two and have been quite succesful but at the moment I am having difficulty with the Z axis while trying to cut 3d.

It seems to step down as if it is missing steps and the cut gradually gets deeper. I have tried everything that I can think of , resetting the steps etc and cleaning and lubricating the Z axis in case it was a mechanical problem, all to no avail. I only seem to have trouble with the 3d carving with 3d machinist.

I wonder if this could be a cv problem on the Z axis. Any ideas at all or could you explain to me how it affects the Z axis?

Roly
From Batlow
Roly
Vectric Apprentice
 
Posts: 73
Joined: Thu Nov 16, 2006 12:17 am
Location: Batlow Australia

Postby metalworkz » Sat Sep 27, 2008 12:41 am

Hi Wingnut,
It almost looks as if the rectangular vectors around the 'Push' & 'Pull' are open vectors? If so it may help to 'close' those vectors up also. What are the other settings in your CV control set too? I use Mach3 with my SX3 mill and the CV Dist tolerance with 180 units and the G10AdaptiveNurbsCV are checked.
Best regards,
Wes
wes.spence@comcast.net
Gingery Machines:
Lathe, Horiz. Mill, Shaper, Leaf Brake
User avatar
metalworkz
Vectric Wizard
 
Posts: 2387
Joined: Mon Mar 31, 2008 3:26 am
Location: Modesto, California 95358 USA
Model of CNC Machine: SX3 CNC, DIY 24x20 & 48x60 routers

Postby wingnut2.0 » Sat Sep 27, 2008 1:30 am

HoustonFirefox,
Thanks so much. I made the changes per your post and all is well. Now my self-assigned homework is to sit down and try understand what CV does as well as this tangential setting. Thanks again.

metalworkz,
Those were not open vectors, but an attempt at tabs. I do not have any other CV settings enabled(see pic). I am using a SmoothStepper and I cannot say enough about how much it has improved the overall performance of the machine. I am running on a laptop(not dedicated to CNC) and initially the machine sounded like I threw a bunch of bolts in a blender, but now I am able to reach rapids I never thought possible. More importantly that the higher speeds is the accuracy. I have re-cut older files and there is a huge difference.

Thanks again to all for the help.
Attachments
genconfig.JPG
wingnut2.0
 
Posts: 5
Joined: Thu Sep 25, 2008 3:20 am

CV explained

Postby ger21 » Sat Sep 27, 2008 3:41 am

http://www.machsupport.com/docs/Mach3_CVSettings_v2.pdf

Tangential settings are for aligning a knife blade to the tool path with a stepper motor.
Gerry
ger21
Vectric Wizard
 
Posts: 312
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: CV explained

Postby HoustonFirefox » Sat Sep 27, 2008 10:00 am

ger21 wrote:http://www.machsupport.com/docs/Mach3_CVSettings_v2.pdf

Tangential settings are for aligning a knife blade to the tool path with a stepper motor.


Gerry, you are absolutely right. Mainly this is if you have a directional X-Acto blade attached to the Z-axis for vinyl cutting :idea:
CNC Woodworkers do it with a 3D Touch Probe!
User avatar
HoustonFirefox
Vectric Craftsman
 
Posts: 216
Joined: Wed Aug 22, 2007 5:17 pm
Location: Houston, TX

Re: Help with engraving

Postby HoustonFirefox » Sat Sep 27, 2008 10:07 am

Roly wrote:Houston,
It seems to step down as if it is missing steps and the cut gradually gets deeper. I have tried everything that I can think of , resetting the steps etc and cleaning and lubricating the Z axis in case it was a mechanical problem, all to no avail. I only seem to have trouble with the 3d carving with 3d machinist.


Roly, I vaguely recall having had this same issue awhile back with Photo VCarve, but it wasn't PVC's fault, it was my settings in Mach 3. Try slowing down the Z axis motor to say, half of what it is now and smooth the Z-axis ramping. You can always speed it up if it works later. Add a few units to the Z-Axis dwell as well if able.

It may be that during the plunge into the work, the Z-axis is losing steps since it has to work harder, retracting, then "adding" those missing steps into the next Z-Axis descent into the work. Try it and let's see what happens. :wink:
CNC Woodworkers do it with a 3D Touch Probe!
User avatar
HoustonFirefox
Vectric Craftsman
 
Posts: 216
Joined: Wed Aug 22, 2007 5:17 pm
Location: Houston, TX

Postby HoustonFirefox » Sat Sep 27, 2008 10:25 am

wingnut2.0 wrote:HoustonFirefox,
Thanks so much. I made the changes per your post and all is well. Now my self-assigned homework is to sit down and try understand what CV does as well as this tangential setting. Thanks again.


Glad the info worked for you. I ran my machine at first for about 4 months with CV mode disabled and went through two X-axis leadscrew nuts that wore out from the constant starting and stopping (not to mention the table hopping around the shop) before I figured it out. Note that I used 45 degrees as my example; I know of others that use 38 degrees and yet another that has better luck with 50 degrees. 45 seems to work for me and my machine but with a gantry that weighs close to 200lbs it wouldn't surprise me. (It's not my design guys!).

Again, glad the info was useful. Play around with CV mode, it's fun to tweak :shock:
CNC Woodworkers do it with a 3D Touch Probe!
User avatar
HoustonFirefox
Vectric Craftsman
 
Posts: 216
Joined: Wed Aug 22, 2007 5:17 pm
Location: Houston, TX

Postby Roly » Sun Sep 28, 2008 6:18 am

Houston,

I realise this is out of topic but still seems to be worthwhile to post it here, Thank you for your advice, I retuned the motor as you suggested halving the speed and dropping the acceleration a bit {also about half}.

Seems to be working a treat. I have been reading posts on cv for awhile and it never occurred to me to slow the motor velocity down and as a result had them running at max speed for them on my machine.

Anyway, thanks again, your suggestion seems to have fixed the problem.

Roly
From Batlow
Roly
Vectric Apprentice
 
Posts: 73
Joined: Thu Nov 16, 2006 12:17 am
Location: Batlow Australia

Postby HoustonFirefox » Sun Sep 28, 2008 4:20 pm

Roly wrote:Houston,

Seems to be working a treat. I have been reading posts on cv for awhile and it never occurred to me to slow the motor velocity down and as a result had them running at max speed for them on my machine.

Anyway, thanks again, your suggestion seems to have fixed the problem.


Roly,

Glad to hear it fixed the problem! I had this issue not only on my Z-axis, but on my X (long) axis on my 4x8 plan-built CNC bed. It seems that the fast travel I was using worked great most of the time, but I had some gantry-binding at the far ends of my X-travel which caused the X to "lose" then "add" those steps when the gantry went back to the area I normally use. A little tuning with a hammer, duct-tape and a paper-clip fixed the issue. :D
CNC Woodworkers do it with a 3D Touch Probe!
User avatar
HoustonFirefox
Vectric Craftsman
 
Posts: 216
Joined: Wed Aug 22, 2007 5:17 pm
Location: Houston, TX


Return to VCarve Pro - General

Who is online

Users browsing this forum: Art Mann, cnc4me, Google [Bot], kacy 49, kenlyall, Mobius and 6 guests