XYZ Axis Starting Point

[Gs.spencer]

Every time I load a new G code, I zero out the XYZ axis (I normally use the center point instead of a corner). Whenever I select "Run", the router bit always drops down to the Z-zero axis point and then lifts up and moves to a new location and begins carving at some other point on the wood. This is just fine behavior and usually isn't a problem.

Is there a way to prevent the bit from sinking down to the Z-zero point after selecting "Run"?

My problem is sometimes I carve on a large piece or 24" x 24" wood and the wood isn't perfectly flat. It's more of a problem when I use a fine 20-degree x 0.020" tip engraving bit and I set my cutting depth real shallow like 0.020" or 0.030". One side of my board the lettering will be a perfect depth but on another side the depth will be way too deep or way too shallow.

My fix for this is to break up my lettering into several smaller TAP files and then I set the Z-zero axis where the carving will be and not set it at the center. This trick works real good except when I select "RUN", the bit always goes back to the center Z-zero point. If I zeroed the Z axis on a different part of the wood and that point is lower than X0Y0Z0, the begining of my carving will now put a small hole in the center of the project.

After setting my Z-zero elevation at a point other than X0Y0, how do I prevent the router from returning to X0Y0Z0 after I select "RUN"?

Thanks, Greg
www.wood-gsco.com

[Eagle55]

Greg,
The blunt answer to your question is NO, you can't stop it from doing what some refer to as the "kiss of death" at the beginning of a carve. I guess you might say, its a "Shark thing". (Actually, I don't know if other brands operate like this too, or not, but the Shark does). Now for the way around the problem, as you have discovered, you can break up your work and do the different zeros more locally to where it is going to carve, but as you discovered, that has its problems. Another way to use that same technique depending on how critical the locations of the various sub-components of your carve is, you can choose to relocate you X/Y zero to that are so that when it dips down to zero, you are ok. But that is a lot of work to accurately change your XY zero setting for several different areas. The other solution is to re-evaluate the over all method/problem. The one most prevalent cause of the problem is that the bed is often not level or sometimes has sags etc. I engrave Corian a fair amount and its hard to tolerate the various depths of engraving that you have discovered... it makes the lettering bolder at one spot than across the material at another spot. What I do on a regular basis is to use a dial indicator chucked up in the router collet and jog across the material to see how far out it is and where. Then with a good idea of how much I need, I place shims on the 4 corners as needed to bring the material very close to parallel with the plane of the router travel. What works good for me is to keep it within plus or minus .005". I don't know how well this will work with .020-.030" carving depth but is works well for me with 1/4" - 1" lettering where I would normally have a problem if I just clamped hard against the bed. Bottom line is that you have to have reasonably close tolerance of material top surface flatness with respect to the plane of travel of the router. It becomes much easier if you have a perfectly flat and level table and put on perfectly uniform thickness of material, but that quite often isn't the case that we have to deal with so improvising becomes the next best thing. Its getting late, so I can only hope that I made sense and didn't ramble on. I'll try re-reading it in the morning and may modify it. LOL

Roger

[drueth]

Greg

Leveling the table to the router would be my first step, But you also could use a large dia end mill bit and plane the board flat befor you start to do your cuts. Depending on which shark model you have and if you have and have you read some of the other post on this site about different issues the board may not be flat when you are done planing it but it will be planer to the router as it travles from side to side and frount to back.

[4DThinker]

Set Z depth at the top of your board, then reSET it to 1/16" above the board in the controller. In Vcarve have your tool paths starting depth set to 1/16".

Now when it homes at the beginning of a cut it'll be 1/16" above the board. Because all your jobs are 1/16" down, they'll all cut as usual.

You can also "trick" it to do this automatically by changing the set thickness of the touch plate to 1/16" less than it really is.

[Gs.spencer]

4DThinker I think you nailed it, that's the perfect solution!!!

Here would be the steps:

1. In V-Carve, set the Start Depth to let's say, 0.050"
2. In "Material Setup" set "Rapid Z" Clearance & Plunge to 0.1"
3. Set your X0Y0 axis point to the center of the board
4. Move the XY axis to the carving point where your board might be a little lower (or higher) than the X0Y0 origin.
5. Lower the Z axis router bit tip to the board and "zero" the Z axis
6. Raise the Z axis to exactly 0.050"
7. Zero the Z axis again

You're now ready to start carving.

The only concern should be, what if the start depth is too deep? There could be a chance that the router bit might drag into the board when it transverses to a new carving point. Step #2 above tells V-Carve how high the router will retract when it transverses to a new carving position. I would imagine as long as your Z1 Clearance is higher than your Start Depth, the bit should should always clear the surface when tranversing to a new carving point.

Greg

[Buc]

Greg,

'Z' Traverse position clearence is controlled in the material Setup section on the toolpath side of Vectric software. See attached snip.

Buc

[Gs.spencer]

Thanks Buc, that seals it!

I modified my steps in my previous post and added a step for checking the Rapid Z Gaps.

I've had my HD Pro Plus for about 10 months now and am still learning new tricks. Thanks everyone for piping in...

Greg
www.wood-gsco.com

[KarenW]

I do a slightly different step to avoid the tiny little divot in the center.
Since I do a lot of work with a depth of cut set at .011 or less, I zero the machine using a .003 feeler gauge. Once the tip of the bit is just scratching the gauge, I reset my toolpath and add the .003 to the flat depth. When I hit 'run', the tip of the bit starts out at the .003 above the surface but my finish depth will be the .011 (or whatever my flat depth is for that project).