VCarve machining with 2 cutters

[hbrannon]

I have followed the instructions from Vectric on machining with 2 cutters and get fairly good results, but my first cutter whether a vbit or and end mill seems to always go slightly deeper than the pocketing bit. This leaves areas around letters, etc unsightly, especially after painting. I have tried cleaning them up with sanding, scraping etc, but this is very tedious. Don't know if its my machine or in the software. Anyone have any suggestions.

[blackhawk]

Are you talking about pocketing around letters?

[hbrannon]

Yes, when I choose vcarve as a tool path and specify a flat area depth and choose an additional tool to clear, I get this problem. Vectric also has a way to do the same by choosing an end mill for the first cut, but telling the software that the end mill is an engraving bit. This allows clearing using two bits, but not having to vcarve or angle around the letters. I get the problem doing this as well.

[blackhawk]

You will never get the two separate cutters to cut perfectly at the same depth. I see this also on my machine. I use Vectric and it is not a problem in the software. It is nearly impossible to get both cutters zeroed perfectly and then have the machine move to depth exactly the same. Here are a couple of things to try. First, when you zero out your V-bit with the zero plate, move your plate slightly when the V-bit comes down to touch off the second time. I found that my V-bit was so sharp that it would make an indentation on the first touch and then on the second touch that sets zero it would go into that indentation setting the zero just a few thousandths deeper. If you still see a step, make note of whether it is always the same cutter that is too deep. For example, if the V-bit is always deeper than the endmill, zero the V-bit as normal with the Z plate. Then do an MZ move to say +.005 and then manually set Z to 0 at this point. This will fudge the V-bit just a little higher. Play with that and you can fine tune it in.

[joe]

Hugh,

There are so many potential reason you are having this problem it's hard to tell. Perhaps you could try some of the following solutions.

Place your Z Zplate in the same place each time.
Zero to the table, not to the material surface.
Ramp into your cuts. Three steps is enough.
If the problem is consistant you can place a business card under the zero plate, or something the same depth as you bad cut.

In the coming Craftsmen Workshop I'll be using business cards, charge cards, coins and other materials when fine tuneing V Cuts. It's called cheating. It's a fast and powerful method to adjust heights without redoing the file.

Good luck,

Joe

[hbrannon]

Brad & Joe,
Thanks for the suggestions, I will try these on some practice projects today. This forum is a fantastic tool, thanks for your involvement.

Hugh

[jhicks]

Hugh, there are several possibilities here. When you set up your V bit in the tool library you basicaly set the diameter and angle,and the software calculates the cut depth or the angle and the cutting lenght and ,the software determines the diameter.
So if what you have is an estimated dimension or the angle is not a true 90 but rather 88 or 91 degrees, your math will be incorrect and calculated from your library settings.
This definately can have an impact on step over lines and actual steps between multiple passes and might also be delivering a slightly different depth of cut.
Some other possibilities are a combination of hold downs and material stress relief. If you have the V cut first, then the area clear, you might be experiencing material cupping as the stress is relieved by the removal of material which could cause you to see different depths.
Multi tool surface machining is quite sensitive to your Z zero plate, zeroing on the exact same spot between bits, material stress relieving, hold down method, and accuracy in your bit library to name a few.
When everything is properly dialed in, you should see very little variation between the changes with the main exception being material movement from stress or marginal hold down. Screwing down for example on corners is OK but depends on the material and Zeroing on the same spot between bits is quite important as wood for example may not have been planed perfectly flat and can cause problems like you describe.
As can the table level surface condition, dust under the part etc.
Good luck, you can get there but need to determine the root cause.

[hbrannon]

Thanks Jerry, hadn't thought of the stress relieving issue, I believe I have been experiencing that on large pocketing areas using a single bit. Thanks for the help.

Hugh

[procarve]

I have had this same problem when v carving the edge and flat milling the center of a cutout. I have also seen it when 3d milling with a small ball and then using a flat cutter outside that area.

I hate to fuss around with these type of really sensitive adjustments so I cheat.

Knowing the little ledge will be there when using a flat mill next to a vcarve or ball nose area, I make it part of the design - set the depth to cut for the flat bit slightly higher or lower and use the ledge as an accent. It can actually look pretty cool when done right. Lots of times I modify my design intent to meet the strengths of the tool and not fight physics.

I will try and dig up a couple photos for illustrating the point.

Bill
www.RocketfuelSigns.com (http://www.RocketfuelSigns.com)