Can someone explain the advantages and disadvantages of referencing the Z off the material surface and also off the machine bed? I’m still waiting for my OF but am trying to do my best learning Vetric. Thanks for your help!
1 Like
My approach has been to zero off the wasteboard when I want to cut all the way through the material and to zero off the material surface when I want to v carve or cut pockets into the material that are relative depth to the material top surface. This approach removes issues with variable material thickness from a repeatable process where you will use the same program to make the same part multiple times.
There may be better ways but this works for me.
5 Likes
I appreciate it very much.
I generally reference off the material if I am not cutting all the way through but I prefer to reference off the waste board if the thickness of the wood varies or may be milled away when changing bits.
3 Likes
I’m very new to this but figuring out the software. My question is, if I zero off the wasteboard, and in VCarve Pro set material thickness to.75 for a “3/4” piece of plywood, will the machine know how to start out with clearances above workpiece. IE I want to cut through, utilize tabs, and not cut into wasteboard. My first attempt to cut out a circle for a vent fan in 3/4” plywood for my CNC table resulted in a slight cut into wasteboard. I selected Profile cut, material top w/tabs and a ramp in. When measuring the plywood thickness it varied significantly as I expected. I chose an average of the thickness’s. I guessed lucky as had I put in .75 for a thickness, there would have been a much deeper cut into wasteboard.Am I on the right track? Through cuts, zero off wasteboard, put a close material thickness? Thanks to anyone answering a very basic question but until you get some experience, these aren’t “no brainers”. I’m just trying to be smart with configurations and maximize wasteboard life.
The clearance distance from the wasteboard will be based from whatever thickness you tell VCarve. i.e., thickness + clearance
If you are working with 2D through-cuts, where depth of cut is not a concern, then you can set the thickness of the material greater than the actual, as long as you cut to the full depth. So, you could set the material thickness to 0.8" and depth of cut to 0.8" in your tool path. This leaves you extra clearance above the material if it’s uneven. If you are doing 2.5D cuts, it’s probably better to zero from the material surface for accurate depths.
If you are using a probe and still cutting into the wasteboard when zeroed from the wasteboard, then you need to accurately measure your probe and adjust the value in the controller settings.
1 Like
Thanks very much. I was doing a 2D cut and your explanation makes perfect sense. I do have a probe as well, just didn’t understand why you would ever set Z to the wasteboard. I’ve probably read every post and topic in the forum, what a great support community! Gotta shout out to 1F for engineering such a great product! I hope in the future to gain the knowledge of others and help newbies like myself in the future.
Brian Lindell
I suspect the main reason is to prolong the wasteboard’s life and keep it looking pretty. That’s why I do.
There are other potential uses too. For example, one could mount their probe at a fixed position if they wanted to automate Z probing.
Depending on the cut type I use both
A lot of my work is full thickness cuts cutting out profiles for this I use the spoil board I zero on the board raise up by 0.1mm, and re-zero this leaves a thin onion skin, it also prolongs the spoil board life and using a down cut bit the onion skin saves any breakout it also means that if the thickness of your timber is slightly out then this doesn’t effect the finished item it just means the first profile cut is either a little heavy or a little light.
If I am engraving or cutting a pocket or well then I usually zero on top of the workpiece this does rely on the workpiece being on size particularly if you are doing a number of the same item.
I run Carveco Marker and in each tool path it allows you to set the clearances and home position,
The home and zero on my machine is bottom left but on most of my jobs the zero is bottom left but the home is top left X0 Y250 this means that at the end of the toolpath the spindle is towards the rear of the machine and far enough away to allow me to safely unclamp the finished item and clamp the next item, when I then start the next job the machine goes to job zero with the cutter above the job before it commences its cut
May seem at bit over the top for one offs but a lot of my work is batch work of around 100 and I normally produce 5 components from 1 piece of timber so having to move the cutter out of the way and move it back or having to power down the spindle and power it back up all adds to the cycle time.
Hope this helps (i did spend my early engineering years in a production machine shop old habits die hard!!!)
D
1 Like
I’m struggling with this after perusing the forums for a few hours. I have a x-50 woodworker with buildbotics controller. I’m using VCarve Pro and trying to setup a toolpath that can be used to repeatedly surface a boards that are approximately 1” thick to a specific thickness. (.75 inches for example).
Seems simple enough (I thought).
I set material thickness to 1 inch and and the z-zero position for the job to “machine bed” thinking I could then use a pocketing toolpath with a cut depth of +.75 inches. To me that makes sense ( cut to +.75 inches above the z-zero position) but apparently the Onefinity post-processor doesn’t honor the z zero position when it’s set to “machine bed”. The preview shows the tool path cutting -.75 deep instead of +.75 above the machine bed/z-zero?
What am I missing? Do I really have to accurately measure the thickness of every board I want to surface and then manually calculate how much material to remove to get to the the desired thickness?
I suppose I could create g-code that runs a raster pattern at a specific z height? Is that how this is done?
Thanks in advance for any guidance you can provide.
If your material can go up to 1” and you always want to surface down to .75”:
- In VCarve:
a) Set material thickness to 1”
b) Set Z Zero Position to the Machine Bed
c) Set start depth of your pocket tool path to 0”. (top of material)
d) Set cut depth of your pocket path to 0.25”.
- On your CNC:
Set Z zero to the machine bed (wasteboard)
Your cut depth is how much you are cutting out, not how much you are leaving.
Example: I want to carve a 1" pocket in a block of wood. I'll use a roughing bit to do most of the work, then a down-cut endmill to do a clean finishing pass.
1) Use a roughing bit to cut to depth of 0.95". (Start depth = 0.0"; cut depth = 0.95")
2) Use the down-cut endmill to cut to final depth of 1.0". (Start depth = 0.95"; Cut depth = 0.05"). I could set start depth to 0 and cut depth to 1, but I would be cutting air for the first 0.95".
1 Like
Thank you… Makes perfect sense now and works great I guess I just needed a fresh perspective.
2 Likes