Finding home.

This forum is for general discussion regarding VCarve Pro
Post Reply
knick58
Posts: 7
Joined: Sat Jul 08, 2017 7:19 pm
Model of CNC Machine: MultiCam 5000

Finding home.

Post by knick58 »

Great software! But I cant find 0,0 on my machine. I've always had 0,0 as the upper right corner of the machine bed. That is where I home my spindle every time. With V Carve I always get an out of bounds message at my machine. Then I have to guess where to home the machine to get my project to run. What am I doing wrong? Other than this issue, the software is pretty easy to use. I have a Multi Cam 5000 CNC.

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Finding home.

Post by Adrian »

The XY datum position is set in the job setup when you first create a job or under the Edit menu under Job Size and Position.

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Finding home.

Post by Leo »

On just about every machine there are 3 coordinate systems.

1) - What you are referring to as "home" on your machine is actually called a "Machine Coordinate" or a Machine Coordinate system. That is where the MACHINE "X" - "Y" - "Z" zero is located. That place may be a different place on different machines.

2) - The Work, or Fixture or Part, coordinate system. That is where the "X" - "Y" - "Z" zero point on the part is located. It is a defined distance, or offset away from the machine coordinate system. That is set in the machine, not in Vectric. This setting in the machine really doesn't have anything to do with Vectric.

3) - IN VECTRIC - the setting to define "X" - "Y" - "Z" in the material setup is the actual zero location on the work, or part. That doesn't "really" have anything to do with the machine at all. This one is the program zero point.

When you are setting the work coordinate position (some people call this touching off), the point that you set MUST be the same point that you set in Vectric.

So There are 3 independent coordinate systems. They are all independent but they do interrelate with each other.

I know it "sounds" confusing and it "sounds" contradictory - but if you think hard enough about it - it makes sense.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5887
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Finding home.

Post by Rcnewcomb »

As Adrian mentioned, you can set the Datum position for the job to any of 5 different positions.
Datum.JPG

You can also edit the post processor to customize it for your preferences. Go to Help /Post Processor Editing Guide and it will bring up a PDF document. You may wish to update the headed and/or footer to have it start and/or end the router in a particular position.
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

knick58
Posts: 7
Joined: Sat Jul 08, 2017 7:19 pm
Model of CNC Machine: MultiCam 5000

Re: Finding home.

Post by knick58 »

Thanks for the replies. I guess I'm thicker than most. So looking at the pic in one of your posts, the hi-lighted XY
datum position refers to the material only. The part will be machined from that point down and left from there? But that has nothing to do with where that starting point is on my machine?

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5887
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Finding home.

Post by Rcnewcomb »

Let's try a specific example.

I drew a square 11x11 on a 12x12x1 piece of material with the datum specified in the upper right and Z-zero on the machine bed.
I did a profile outside the square at a depth of 0.1.
I used the MultiCam G Code Arc Inch post processor and it generated the following code.

What do you want it to do that it isn't doing?

Code: Select all

M90
G90
G17
G70
G74
G00T1
G97S12000
G00Z-1.8000
G00X0.0000Y0.0000
M12
G00X-0.3750Y-0.5000Z-1.2362
G01Z-0.9000F0.5
G03X-0.5000Y-0.3750I-0.1250J0.0000F1.7
G01X-11.5000
G03X-11.6250Y-0.5000I0.0000J-0.1250
G01Y-11.5000
G03X-11.5000Y-11.6250I0.1250J0.0000
G01X-0.5000
G03X-0.3750Y-11.5000I0.0000J0.1250
G01Y-0.5000
G00Z-1.2362
G00Z-1.8000
M22
G00X0Y0
M02
Attachments
multiCAM.crv
(23 KiB) Downloaded 58 times
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

knick58
Posts: 7
Joined: Sat Jul 08, 2017 7:19 pm
Model of CNC Machine: MultiCam 5000

Re: Finding home.

Post by knick58 »

I appreciate your effort, but see if you can answer my questions if they make any sense at all about your example.
1. The datum on the material is where the router will start machining the piece? Yes or No
2. The machining would start , in your example, in the upper right corner and machine left and down from the datum point? Yes or No
3. How does the datum point relate to Z zero? Don't understand that at all. Z is up and down. X and Y would locate a point on the machine bed.

I will stop there for now. Thanks a bunch for your help.

User avatar
highpockets
Vectric Wizard
Posts: 3667
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Finding home.

Post by highpockets »

The machine "home" is most of the time different from the datum point specified in VCP.

When you tell your machine to set "home" it moves to a spot that sets up the X0 Y0 Z0 for the machine.

When you place a piece of material on the machine you then move the XY axis to the point on the material that you setup as the datum point in VCP and "zero" the XY DRO (Digital Read Out) of your machine. To set the Z axis, after installing the bit you need move the Z axis down to were the bit just touches the datum point you set for the Z axis (either the top of the material or the top off the machine bed). Then set Z DRO to zero.

Hope this helps.
John
Maker of Chips

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5887
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Finding home.

Post by Rcnewcomb »

When you are standing in front of your machine like this....
Image
You prefer to have the spindle start and end at the back, right corner, correct?

I assume that if you send your machine to X 0, Y 0 then the spindle moves to the front, left corner, correct?

Assumin gyou have a 48x96 table I think what you want to do is on the Toolpath Material setup screen tell it Home/Start is X 48, Y 96
HomeBackRight.JPG
It really doesn't matter where you have the Datum set.
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

User avatar
sharkcutup
Vectric Wizard
Posts: 2885
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Location: U.S.A.

Re: Finding home.

Post by sharkcutup »

I'll try giving this a Go :-)

XY Datum Position

This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that
will match the machine tool when it is positioned at X0, Y0.

Think of it like this:

Your Design (V-Carve G-code Data File) and the machine (Control Panel Software) carving start positions (X, Y, Z) must match in order to produce
an acceptable product.

After clamping down your material this is achieved by jogging each axis X, Y, Z, to the same XY Datum (5 positions to choose from - center or
the four corners) ZERO POSITION and Z POSITION (top or bottom of material) as set in your V-Carve design.

Example:

(V-Carve Software) --- I have a design where I want to carve a 6" by 6" square in a 12" x 12" Material Board. In my Material setup I
have the Z Zero Position set to the top of the material and the XY Datum set to the center.

(At the machine) --- I have my 12" x 12" material board clamped down to the center of the machine table bed. Before I clamped the material board down I located
the center of the material board and marked it. I now know where to set my machine XY Datum ZERO Position and the Z ZERO Position in same relations to my V-Carve design.
I first jog the machine X and Y axis to the marked center of the material board once there I click the appropriate X and Y buttons at the control panel
software which changes the numbers noted there to ZERO. I then gradually lower the bit to the material with piece of paper between bit and
material until the bit just touches the paper and it can move freely between the bit and material. I then click the appropriate Z button at
the control panel software which then changes the numbers there to ZERO.

The Machine X,Y,Z Zero now matches my design software g-code file X,Y,Z Zero. They are now identical and should produce an acceptable product.


The Home/Start Position

This is the absolute position that the tool will start moving from and where the tool can be programmed to return to at the end of cutting the
job.

Think of it like this:

This is where you want to have your spindle/router at the beginning of a project, return to this position at the end of the carving operation and
any bit changes during the project.

Hope this Helps explain the XY Datum and the Home/Start Positions! :)

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Finding home.

Post by Leo »

You can read my post earlier in this thread.

It might help - or it might not.

I work with CNC for a living, Lots of machines and in many different companies. They all work the same way.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
sharkcutup
Vectric Wizard
Posts: 2885
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Location: U.S.A.

Re: Finding home.

Post by sharkcutup »

From Leo
You can read my post earlier in this thread.

It might help - or it might not.

I work with CNC for a living, Lots of machines and in many different companies. They all work the same way.
Not trying to undermine your earlier post. I was just trying to put information out there in another manner.

I have followed many of your posts due to the fact they seemed (which you have just clarified) to be very experienced and professional posts. Your posts along with several other individuals here on this forum are very educational and informative. I have learned a lot from browsing this forum.

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Finding home.

Post by Leo »

Shark,

I was not posting about your post, but more the those asking the questions. You did a fine job on your post, very clear and concise. Sorry for making it sound like I was criticizing you.

Someday, I will create a video explaining the Coordinate systems. Trust me when I say, I have met machinists and engineers that do not have a clear understanding. I have taught this stuff to a lot of professionals
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
sharkcutup
Vectric Wizard
Posts: 2885
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Location: U.S.A.

Re: Finding home.

Post by sharkcutup »

Thank you for the compliment!

I have used a CNC machine before for inspection of machined parts along with PC-DMIS Software programming CNC inspection machines from CAD models. So I am experienced with how the system is supposed to function.

Videos --- I have thought along those same lines recently too!!!

Have a GREAT DAY!!!

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

knick58
Posts: 7
Joined: Sat Jul 08, 2017 7:19 pm
Model of CNC Machine: MultiCam 5000

Re: Finding home.

Post by knick58 »

Blink! That is the sound of the light coming on! Thanks for your patient and helpful explanations.

Post Reply