engraving numbers with the wrapped output

This forum is for general discussion regarding VCarve Pro
Post Reply
svenko
Posts: 13
Joined: Thu Sep 22, 2011 2:39 am
Model of CNC Machine: Homebuildt Router

engraving numbers with the wrapped output

Post by svenko »

I'm still working on getting my wrapped output working correctly, using VCP 8.5, on my machine dial project with 100 ticks and ten sets of numbers, I now have the tick marks working perfectly with equal spacing but the minute is starts on engraving the numbers it slow to a crawl, I suspect it's because of all the G1 moves and I have found no way to get it to use G2 or 3, I have tried all the different toolpaths and many different fonts. Is the wrapped format limited to G1?, is there a preferred font, TT or single line?. I hope someone will answer my questions so I can get past all this testing and searching.

User avatar
IslaWW
Vectric Wizard
Posts: 1398
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: engraving numbers with the wrapped output

Post by IslaWW »

You do not have the feedrate for your rotary axis set properly
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

svenko
Posts: 13
Joined: Thu Sep 22, 2011 2:39 am
Model of CNC Machine: Homebuildt Router

Re: engraving numbers with the wrapped output

Post by svenko »

I'm using the same tool and and feed rate for the numbers as for the tick marks which works as expected, I'm doing both with a profile toolpath, it's single line lettering, it appears to be a problem with engraving the zero's, I haven't counted the lines of code for the numbering but it's pretty long. Is there something in the motor tuning that I should check ?

User avatar
IslaWW
Vectric Wizard
Posts: 1398
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: engraving numbers with the wrapped output

Post by IslaWW »

A few questions:
1) What controller are you running?
2) What feedrate do you have the rotary axis set to?
3) Does your controller support "G93" Inverse Time Mode?

To set a surface feedrate equal to XY feedrates the formula is: 115* feedrate/diameter. For example, 115 * 100ipm /2 in diameter is 5750 degrees per minute. Sounds fast, but it is only ~16 revs/min or one revolution every 3.75 seconds. I often set rotary axis rapids at 72,000*/min, maybe 36,000 if using higher reduction

Your tickmarks appeared to cut "normally" most likely because they were single axis movement using the unwrapped axis. Once you start on the test the linear axis is being held up by a (most likely) extremely slow rotary feedrate.

Wrapped rotary cutting does not support G2/G3 arcs.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

svenko
Posts: 13
Joined: Thu Sep 22, 2011 2:39 am
Model of CNC Machine: Homebuildt Router

Re: engraving numbers with the wrapped output

Post by svenko »

Hi Gary,
Thanks for the reply, I'm not getting emails notifications, I'm pretty sure I requested that, anyway just saw your post. I'm using Mach3 I have a standard 200 - 1.8 degree stepper and 7.2 reduction on the timing belt drive. My settings are 40 steps per degree 12186 velocity and 1000 acceleration. I was not aware of the formula that you list and will be trying that as soon as possible, certainly sounds like that's where my problem lies. Thanks for help it's very much appreciated. Svend

svenko
Posts: 13
Joined: Thu Sep 22, 2011 2:39 am
Model of CNC Machine: Homebuildt Router

Re: engraving numbers with the wrapped output

Post by svenko »

Sorry I forgot to mention the 10 micro steps .

svenko
Posts: 13
Joined: Thu Sep 22, 2011 2:39 am
Model of CNC Machine: Homebuildt Router

Re: engraving numbers with the wrapped output

Post by svenko »

Hi Gary, I did some research on the G93 Inverse Time Mode and it appears that it is supported by Mach3, it is listed in the Mach3 Mill G Code summary and gives a brief description of it's function but no examples of how to implement it, if you know of a source where I can familiarize myself with it I would appreciate the link. Again thanks for all you help, Svend

User avatar
IslaWW
Vectric Wizard
Posts: 1398
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: engraving numbers with the wrapped output

Post by IslaWW »

Sorry Svend…
I have no information pertaining to Mach, maybe others will chime in.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: engraving numbers with the wrapped output

Post by ger21 »

You don't need to use G93 with Mach3.
But here's what you need to do:
1) Go to Config > Toolpath, and check "Use Radius for Feedrate".
2) Go to the Settings page, and enter the radius of your part in the Rotation Radius DRO.
3) Make sure you set Z zero to the center of rotation.
Gerry - http://www.thecncwoodworker.com

svenko
Posts: 13
Joined: Thu Sep 22, 2011 2:39 am
Model of CNC Machine: Homebuildt Router

Re: engraving numbers with the wrapped output

Post by svenko »

Thanks Gerry I'll try that tomorrow.

Greolt
Vectric Wizard
Posts: 990
Joined: Fri Sep 21, 2007 1:44 pm
Model of CNC Machine: UCCNC Router, Plasma, Laser
Location: Australia 3781

Re: engraving numbers with the wrapped output

Post by Greolt »

Just to add to Gerry's info,

If you want to have Z axis origin on the outer diameter of the cylinder rather than the center of rotation,

then enter the radius value in the "Rotation Radius DRO".

Or more correctly, the amount that the Z axis origin is above the center of rotation.

Mach3 needs to know where the Z axis origin is, so that it can compensate the rotary axis velocity correctly.

Having said that my preferred method is as Gerry said.

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: engraving numbers with the wrapped output

Post by ger21 »

Greg, I think I what I said was wrong. If the Z origin is at the center, then leave the radius setting at 0, or 0.001. Correct?
Gerry - http://www.thecncwoodworker.com

svenko
Posts: 13
Joined: Thu Sep 22, 2011 2:39 am
Model of CNC Machine: Homebuildt Router

Re: engraving numbers with the wrapped output

Post by svenko »

You were both saying the same thing "set the radius value in the Rotation Radius DRO". I think what Gerry is saying about it being zero makes sense. I ran a bunch of test mostly with the same radius but then my final job was about 1" larger diameter and I forgot to change the Rotation Radius in Mach but I did set my Z center at the center of the part and it turned out well as you can see in the attached picture. The last digit cut was the middle one between the ten and zero marks. It would be more convenient to set zero on the top of the part or does someone have a slick way of using the probe to set the center. Thanks to all of you that posted here, your help is much appreciated. Svend
Attachments
IMG_0563.JPG

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: engraving numbers with the wrapped output

Post by ger21 »

You can set Z zero to the surface, but then you MUST enter the radius of the part. This should work the same way with the radius = 0 and Z at the center.
Gerry - http://www.thecncwoodworker.com

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5864
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: engraving numbers with the wrapped output

Post by Rcnewcomb »

does someone have a slick way of using the probe to set the center
You can measure your tailstock. The center will always be in the same place. You could use a V-bit and line the V-bit tip to exactly meet the point of the tailstock.
If the point of the tailstock is 4 inches above your table surface, then the center of your rotary material will always be 4 inches above your table surface.

Write the number down on a piece of paper, save it as a custom cut, or whatever methods works for your machine so you can always set the Z to that exact height.
If you have a track for your rotary then the X or Y will also always be in the same place.
If you have holes drilled for your headstock then your X,Y, and Z origin will always be the same for all your rotary jobs.
Attachments
RotaryIMG_20180612_175515902-640x480.jpg
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

Post Reply