v-inlay technique problems

[bking1836]

Hi everyone,

While I have had decent success with V Carve's built-in inlay toolpaths, I also need to use the v-inlay technique for finer details that require sharp corners. And I'm having a problem. For the most part the male pieces are coming out well and "fit" ok in the female pockets. But as you can see in this close up, something is off. I am not getting sharp corners, and it's almost like the v bit is slightly dogboning the corners. The straight portions machined quite well and are a good fit for the male parts.

31267

I am using a 60 degree v bit for both cuts. Female pocket machined to .15" flat depth using the v-carve toolpath with a 2% stepover to clear out the pocket. Male parts are mirrored, offset outwards .18" and then v-carved at .1 start depth and .1 flat depth to create inverse parts.

Any ideas?

Thanks!
Brian

[steve_g]

Brian…

In my experience, this generally means that something isn’t as described to the software… either the 60° V-bit isn’t a true 60° or Z-zero is off.

SG

[bking1836]

Brian…

In my experience, this generally means that something isn’t as described to the software… either the 60° V-bit isn’t a true 60° or Z-zero is off.

SG

Thanks Steve! I fear it is both... A slightly off z zero makes sense to me, as that could cause the bit to plunge (or retract I guess) in the corner too early or too late, which could explain the little bite out of the corners, right?

I don't fully understand how a discrepancy in the v bit angle could cause this issue, but I got a similar response in the Vectric forum.

[steve_g]

Brian…

Just for grins, draw several 1” square vectors, V-carve the first one with a 60° bit defined as a 60° bit, define a new bit as 61° and cut the second with the same 60° bit but with the 61° definition then 59° etc. See if you get sharper corners with another of the definitions. It’s not unusual to find that the bit is off…

SG

[bobmoore]

It looks to me like your machine is bouncing a little when it changes direction. check that everything is tight in all 3 axes.

[Red F]

I agree with Steve that the bit angle looks off slightly.

[bking1836]

Brian…

Just for grins, draw several 1” square vectors, V-carve the first one with a 60° bit defined as a 60° bit, define a new bit as 61° and cut the second with the same 60° bit but with the 61° definition then 59° etc. See if you get sharper corners with another of the definitions. It’s not unusual to find that the bit is off…

SG

Good experiment. I will give it a try. In the Vectric forum someone suggested that my V bit's tip might have worn down to a slight flat tip rather than a point, and that could also cause this. I still can't wrap my head around how bit geometry discrepancies can lead to this particular result, especially since the male pieces machined correctly. But spacial reasoning isn't my strong suit...

As for Bob's suggestion that my machine could be bouncing around, I'm not sure how to look into that. It's still less than 6 months old and otherwise cuts as expected.

[Brady Watson]

As for Bob's suggestion that my machine could be bouncing around, I'm not sure how to look into that. It's still less than 6 months old and otherwise cuts as expected.

Turn the control box on and wiggle the living daylights out of it in ALL DIRECTIONS. Grab the spindle force it by hand up and down. Front and back. Left and right. Feel or hear slop? Find it. Same with the X/gantry @ EACH side. Same with the YZ car.

Have a PRS? Check the lower v-roller bearings. Remove the black covers and adjust...not too tight...not too loose.

-B

[bill_l]

Brian,

I agree with Brady. Way back when I had similar results when VCarving. Turns out that the Z axis pinion was not seated far enough on the stepper shaft and was binding near the top of the travel. When VCarving into corners the bit retracts while still moving in the X and Y. If Y lags due to binding or slippage you get what appears to be overcut. Do as Brady said and I think you will find the solution.

Bill

[bking1836]

Brian,

I agree with Brady. Way back when I had similar results when VCarving. Turns out that the Z axis pinion was not seated far enough on the stepper shaft and was binding near the top of the travel. When VCarving into corners the bit retracts while still moving in the X and Y. If Y lags due to binding or slippage you get what appears to be overcut. Do as Brady said and I think you will find the solution.

Bill

Ok thanks Bill and Brady. I will look into this.

[scottp55]

Having a Small flat on the bit won't make that much difference...Most of my VInlays were done with an Onsrud .25"shank 60degree engraving bit with a .01" flat defined as a VBit in the toolpath, they came out fine.
I agree with Brady...looks like something is loose/binding somewhere.
scott

p.s. Why the offset in the Male?

Oh...JUST saw on Vectric forum that you're using an offset vector as a boundary box:)

[bking1836]

Ok....So I think the gantry sits on the X axis tightly. And the spindle doesn't budge. When I yank on the yz car from the side by pulling near its bottom, it is tight. But when I yank on the yz car from the side by pulling near the top (by the plastic cable car), which is closest to the rack and pinion, I think there's a little bit of slop. At least it's the only place I've yanked on the machine and felt movement.

So what does that mean? Thanks so much for your help!

BTW, beautiful inlays Scott. That's what I am hoping for!

[phil_o]

Turn the control box on and wiggle the living daylights out of it in ALL DIRECTIONS. Grab the spindle force it by hand up and down. Front and back. Left and right. Feel or hear slop? Find it. Same with the X/gantry @ EACH side. Same with the YZ car.

Have a PRS? Check the lower v-roller bearings. Remove the black covers and adjust...not too tight...not too loose.

-B

After reading this advice for checking for slop I performed this test on my machine. I have a 12 year old PRT benchtop. When I push on the gantry that travels in the X direction I have some noticeable slop, about .02" measured with a dial indicator. How much slop is acceptable, what is the fix?

[bking1836]

Well, I think I have my answer. After tugging on the machine more I can't say I feel much of any slop. So I cut a bunch of squares defining the 60 degree bit's geometry differently for each of them, and they ALL had the same extra scooping out at the corners. So I looked at the bit more carefully and see now that it's probably rounding at the tip. Then I ran the original v inlay pocket toolpath using a newer 90 degree v bit, and presto, sharp corners.

31295

Is it possible that my z zero plate is contributing to the dulling/rouding of v bits?? I cringe every time I watch that point hit the metal plate...

Thanks everyone.
Brian

[steve_g]

Brian…

I know for a fact that I’ve broken the tip of a 30° v-bit while z-zeroing… a 30° bit is a lot more fragile than a 60° bit though.

What I do:

I loosely hold up one end of the plate a bit while the zeroing procedure does its rapid “down” move and then let it lie flat for the second, slower touch. I haven’t had any issues, even with 30° bits using this procedure.

Talking bits… my experience with 60° bits is that the CMT laser point 3 flute bit is unsurpassed in in quality and reliability. It comes to a true point that is dead on concentric. Also, I think that the 3 flute design gives better support to the fragile tip. I’m sure others will dispute or say they have a better solution, but this is my experience…

SG

[kaetamer]

You might try using brass as your zeroing material. Tough to imagine brass dulling or breaking carbide tips...