Help with Rapid Z, Plunge, and Home/Start Position in VCarve

This forum is for general discussion regarding VCarve Pro
Brady R
Posts: 1
Joined: Fri Aug 31, 2018 6:12 pm
Model of CNC Machine: Shapeoko XXL

Help with Rapid Z, Plunge, and Home/Start Position in VCarve

Post by Brady R »

Hello! I recently bought a Shapeoko XXL and have been doing some smaller projects with mostly success. The problem I am currently running into is figuring out my Z1 (Clearance), Z2 (Plunge), and Home/Start position areas with VCarve Pro 9.5. I’m pretty sure I understand what each one does, it’s just how they work together that is puzzling me. I just purchased some larger hold down clamps that require at least 1.75" of Z clearance and when I put that into the Z1 for clearance, the program automatically populates my “Z gap above material” with that number plus 0.01". So if I enter 1.75" in Z1, 1.76" gets put into “Z gap above material” and throws off the cutting depths. After I zero and press start, the machine will retract and hit the upper limit switch, then plunge WAY deeper than what I set it at for flat depth. Seems no matter what I do, they are related to each other and I can’t change one without affecting the other.

My ultimate goal is to be able to set a safe Z height (Rapid Z gap) that will clear my clamps and be able to adjust my Z gap above material independently. Is that something that Vcarve is capable of? Have any of you ran into this problem?

Specs: Machine- Shapeoko XXL
Software- Vcarve Pro 9.5
Machine Z Clearance: 3"

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by adze_cnc »

Brady R wrote:1.75" of Z clearance and when I put that into the Z1 for clearance, the program automatically populates my “Z gap above material” with that number plus 0.01". So if I enter 1.75" in Z1, 1.76" gets put into “Z gap above material” and throws off the cutting depths.
Normally I'd point someone to the help within the program but it appears to be woefully inadequate in describing that whole "Material Setup" dialog.

My immediate question is what do you mean "throws off the cutting depths". Cutting depths for toolpaths should not be linked at all to z1, z2, or the home position "z gap above material". If your machine is doing else-wise I'd suggest it's a problem with the machine control software.

Cutting depths specified in toolpaths will be "0 minus depth" if Z-Zero is at the material surface and "thickness - depth" if Z-Zero is at the machine bed---but the program will take care of that for you.

"Z Gap above Material" or more accurately "Z home" should be equal or greater than Z1 which is why the "automatic population". Your original "Z Gap..." was less than your new Z1. Really the software should set them equal.

This is a long-winded prelude to:

Z Gap... = home position of the machine when you tell it to "go home" when finished
Z1 = height the bit will travel at moving from path to path (clearing clamps in your case)
Z2 = height the bit will start moving downward at the toolpath-specified plunge rate (after having travelled at your machine's maximum rate from Z1 down to Z2).

e.g. Z1 = 1.75"; Z2 = 0.125"; max machine plunge = 150 in/min; toolpath plunge = 20 in/min

travel from Z1 to Z2 at 150 in/min then travel from Z2 to cut depth at 20 in/min.

At least this is all how I interpret things. Clear as mud?

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: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by Adrian »

The Z Gap Above Material (Home Z) is always set to be bigger than the Z1. That shouldn't be affecting your cut depths though as it's nothing to do with the cut depths etc. It's just the position that the Z will go to at the beginning and end of the job (if your Post Processor is setup up that way, most are).

As soon as you hit your top stop all bets are off as to where the machine will move to at that point as where your control software thinks the Z is and where it actually is are two different things as it will have lost steps hitting the top stop.

You have to take into account the length of the bit when considering Z retracts. If you've got 3" of Z movement and a bit that stick out by 2" then any move upwards of an inch or more is going to give you problems. The best solution is to have a switch at the top of the Z which sets the movement allowed automatically. That's how I set my machine up.

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by martin54 »

One other thing that I couldn't see mentioned is if you are altering these settings on an existing file then you need to recalculate all the toolpaths after making the changes, you do get a pop up warning telling you to recalculate so make sure you do.
As Adrian has said if your hitting your upper limit/homing switch then you simply don't have sufficient z clearance for the settings you are using, I have very little z movement as my machine was basically designed for work which involves work with relatively thin materials. I therefore try to look at hold down methods which don't use large clamps sticking up above the material surface :lol: :lol:

ElevationCreations
Vectric Craftsman
Posts: 180
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by ElevationCreations »

I would suspect you are losing steps on Z exceeding the machine capacity.

Are you referencing Z0 on top of material or from the Bed?

garylmast
Vectric Wizard
Posts: 1580
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by garylmast »

The last CNC machine I got, I decided to go with servo motors instead of stepper motors, mainly because on an older one I had to install a larger, double torque stepper motor to control the Z-Axis and servo motors were suppose to be more reliable. The larger stepper motor did solve the unexpected Z-drop. However, on the newer machine, when I first turn it on, I have to wait to hear a "click" at the Z-servo motor before I do anything else. About every 10th time when I turn it on, instead of clicking it will drop and drive whatever mill I left in the spindle through the spoil board, so I got in the habit of putting a block under it before I turn it off. I then have to power off and on to fix it. I still haven't figured out if it's the servo motor controller or the servo motor itself, or something else. So far I continued to screw with it, but one day I'll have to figure out what's causing it and replace the defective part. This problem is not caused by the Mach 3 controller.

Gary

User avatar
wmgeorge
Vectric Craftsman
Posts: 288
Joined: Sun Nov 23, 2008 6:12 pm
Model of CNC Machine: Workbee 1000x750 Mach 4 PMDX Controller

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by wmgeorge »

Here is the problem in Mach3, if you use STOP the remaining gcode for the file your running stays in the buffer, and I am using ESS Ethernet so I think it can be adjusted to a larger size? Its still there so when you restart your file or gcode the buffer runs the rest of that code. It happened to me 2 times before I figured out. If you use Pause it runs that buffer out and then Stops the machine and on mine also the Spindle. I am guessing thats the running the bit into the spoil board, and that has happened just once on mine.

garylmast
Vectric Wizard
Posts: 1580
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by garylmast »

Here is the problem in Mach3, if you use STOP the remaining gcode for the file your running stays in the buffer, and I am using ESS Ethernet so I think it can be adjusted to a larger size? Its still there so when you restart your file or gcode the buffer runs the rest of that code. It happened to me 2 times before I figured out. If you use Pause it runs that buffer out and then Stops the machine and on mine also the Spindle. I am guessing thats the running the bit into the spoil board, and that has happened just once on mine.
My version of Mach3 is over 14-years old, so it may act or appear different then your version. I don't have a Pause button, but I do have a Feed Hold button,which I've never used. What you're describing about the Buffer and Rewind has never happened to me if I Hit the Stop button. However, if I hit the Emergency Stop on the Machine, Mach 3 will continue running, so if that happens, I usually Rewind or use the Run From Here button. I would also have to start the spindle first before hitting the Cycle Start button.

The Z plunge on the older machine was caused by too small of stepper motor. The problem I have on the newer machines is more likely a defective servo motor, but as I mentioned could be servo motor controller. The Drop happens before I even turn on the computer, so that eliminates Mach3.

Gary
Attachments
Capture.JPG

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by IslaWW »

Brady R wrote:Hello! I recently bought a Shapeoko XXL and have been doing some smaller projects with mostly success. The problem I am currently running into is figuring out my Z1 (Clearance), Z2 (Plunge), and Home/Start position areas with VCarve Pro 9.5. I’m pretty sure I understand what each one does, it’s just how they work together that is puzzling me. I just purchased some larger hold down clamps that require at least 1.75" of Z clearance and when I put that into the Z1 for clearance, the program automatically populates my “Z gap above material” with that number plus 0.01". So if I enter 1.75" in Z1, 1.76" gets put into “Z gap above material” and throws off the cutting depths. After I zero and press start, the machine will retract and hit the upper limit switch, then plunge WAY deeper than what I set it at for flat depth. Seems no matter what I do, they are related to each other and I can’t change one without affecting the other.

My ultimate goal is to be able to set a safe Z height (Rapid Z gap) that will clear my clamps and be able to adjust my Z gap above material independently. Is that something that Vcarve is capable of? Have any of you ran into this problem?
You are making the mistake in thinking that the software can intuitively know when the tool is over your clamps. As stated above, The "Z1 (clearance)" is the height that the tool will lift to EVERY time there is a retract. Between toolpaths AND between multiple passes of a given toolpath.

The "Z2" setting is ONLY used on machines that have the "RAPID_PLUNGE_TO_STARTZ" enabled. This allows you to use a higher clearance setting AND a slow plunge rate and lowers the Z from the Z1 to the Z2 at rapid rate to save time. You must be careful using this feature if you have small steppers, as the shift from rapid to feed on the Z can cause loss of steps

The "Home/Start" position is simply a position that you select that you wiah your file to start from. I would propose that it is named incorrectly, that it should simply be named "Start position. Starting from 0,0 when at the lower left corner may cause the bit to travel over the clamps. If you set the start position in the center of the material, the bit will be contained inside the cutting area and seldom if ever travel over a clamp. Try it!

Remember this is simply an option to determine where the file starts from and has NOTHING to do with anything called "Home" or any XY or Z zero, referrence or datum. See below how I would set for an 18" square material block:
Attachments
Z Gaps.JPG
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
wmgeorge
Vectric Craftsman
Posts: 288
Joined: Sun Nov 23, 2008 6:12 pm
Model of CNC Machine: Workbee 1000x750 Mach 4 PMDX Controller

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by wmgeorge »

Gary I have a different screen setup so mine shows Pause instead of Feed Hold but its the same function it stops the machine After it runs the buffer out. With my mishap I think it happened when a file started as the spindle was running full on.


Back to Mach3 and raising the Z before Home to clear clamps. I guess I am a little confused, I thought it could be setup in Mach3 to do it ALL the time.

Yes I try to use Center as Origin point just for the reason of clearing clamps. And renaming to Start point is a darn good idea.

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by IslaWW »

Bill...
For the most part your controller will just follow the code that it is given. So, if you wish that the head is at full retract at ANY time during the file, simply add the appropriate code to the post processor. For most machines this would be one of the many variations of "G0 G53 Z0"


On modern controllers pressing Pause, Feed Hold or Tool Check will immediately pause motion. Each have some minor differences, but you can assume an immediate stoppage of motion. And an immediate resume of cutting once the proper button (cycle start, run, etc) is pressed. You need to remember you are working with stuff that is at least a decade with no development, read as no OEM or user input. That means that anything that has been improved in the CNC world for the last decade, may not be supported.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
wmgeorge
Vectric Craftsman
Posts: 288
Joined: Sun Nov 23, 2008 6:12 pm
Model of CNC Machine: Workbee 1000x750 Mach 4 PMDX Controller

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by wmgeorge »

Yes Gary I understand that Mach3 is outdated (but with 1,000's of users worldwide) and I should update my system to a new desktop running Windows 10 Pro. Then purchase WinCNC the PCI cards and software are perhaps 2k so I will have $3,000 USD in my CNC Router. Did I mention I this was a sideline business / hobby? Even as I already have close to 9k in the machine, plus about maybe another 10-12k in my lasers I think I have invested enough. This is not counting the rest of my shop, and shooting sports hobbies. :D

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by IslaWW »

Bill...
I was not suggesting that you upgrade, simply stating the differences between the controls of yesteryear and todays stuff. I'm thinking you are a good bit off on your numbers tho. One, I think you are vastly underestimating the number of Mach users, I'm thinking way closer to a million. Heck, the Chinese throw 10K copies a year in the US market alone.

You are also exaggerating the perceived price of WinCNC. Small machines have a lower licensing fee, so you could purchase a complete setup, plug and play with a 25 pin cable including a WinCNC supported PC for under $2k. But I would not suggest that for most Mach users, as a rule they seem to be a bit frugal, especially with not wanting to spend good dollars for good control computers.

For hobby and DIY use, I would suggest the Centroid Acorn as the best full featured controller for those on a budget. The hardware kit, Controller, power supply and all cables are under $300. Myself and others have been purchasing refurb Lenovo Tiny PC's loaded with Win10 for $150 to $250 depending on SSD, wireless and other options. they work very well. Licensing wise, they have a file size limited free version and a couple upgrades, depending on where and what your needs are. Specific versions for Mills, Routers and Lathes. And a DIY forum attended often by factory techs and programmers.

The price is the same as mach if you purchase a supported IO board. There have been over a thousand converts in the last year. Its a few bucks more than UCCNC which seems to be a Mach clone. Also seems to suffer from a number of the speed, arc and accuracy issues mach did. Maybe too good of a clone. They claim to have a good trajectory planner, but it is nowhere near Centroid or WinCNC.

Anyway, if what you have is working, then you are good to go. I was just trying to let you know you don't have to deal with the idiosyncrasies of legacy control unless you want to.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
wmgeorge
Vectric Craftsman
Posts: 288
Joined: Sun Nov 23, 2008 6:12 pm
Model of CNC Machine: Workbee 1000x750 Mach 4 PMDX Controller

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by wmgeorge »

Gary I Am considering the Acorn if I have issues with what I have now. I can build a computer if needed rather than use a consumer grade one. I have installed and used SSD system drives for years.

User avatar
wmgeorge
Vectric Craftsman
Posts: 288
Joined: Sun Nov 23, 2008 6:12 pm
Model of CNC Machine: Workbee 1000x750 Mach 4 PMDX Controller

Re: Help with Rapid Z, Plunge, and Home/Start Position in VC

Post by wmgeorge »

I think the Mach software was the pioneer of PC based control systems 2001.

Post Reply