V Carve Inlay issue

[coopcnc]

Simulation Preview

I've had marginal success doing inlays using a 60 degree V Bit. I'm working on a project for my wife and tried this monogram R on some MDF using settings I've gleaned from some YouTube videos, namely .2 DOC for the main recess and .1 start depth with .1 DOC for the 'plug'. However, on the plug the letter is erratic along the edges of the main letter although good on the recess. It appears to not be adjusting laterally for the differing depths needed when passing near other parts of the design although it looks good on the simulation preview. I'm sure it's me, but I have no clue on how to fix it. Any suggestions are deeply appreciated.

[Rcnewcomb]

It looks like some variability in the Z axis.
What is your holddown method for the material?
What is your feedrate for XY and for Z?

[coopcnc]

It's clamped down securely, no movement noted. XY is 70 inches/min and Z is 40. I have the Shapeoko 3 with HDZ upgrade. I looks more like an issue with nearby objects that it's moving up to clear but thereby decreasing the effective radius of the V bit.

[Rcnewcomb]

If the uneven edges aren't visible in the preview then you are dealing with a problem during machining.

60 degree V Bit

Does it come to a sharp point, or does it have a rounded or flat tip?
Have you validated that it is a 60 degree bit, and not 59 ot 61, or even 90 degree?


Can you post your CRV file? If it is too large you can upload it to drive.google.com and share the link.

[ElevationCreations]

As others have stated, check the angle of your V-bit. Also check your machine to ensure proper belt tension, the pulleys are tight on the stepper motors, machine squareness, bed flatness.

Other things to check and experiment - Your Z height & where you are touching off, feed rate on V-carve, and plunge feed on Z V bit. I see a number of issues with the cut MDF piece, not just one item as the root cause.

On your machine keep in mind that the HDZ is a great upgrade, however unless everything is perfect with the machine setup .3" DOC in most materials is alot to ask out of the SO3 with the standard spindle, so you need to find your sweet spot for each tool-path.

Are you using V9.x or V10 VCP?

[coopcnc]

I've attached the CRV file, it is using Aspire 10.012. The bit is a Whiteside 1550 60 degree V-bit. I've not actually measured the angle but my understanding they are good bits and the tip is quite pointed. Max DOC is .2 which seemed common across all of the tutorials I've seen. The recess portion came out perfect which is adding to my confusion. The picture does have other issues but that is largely due to me tweaking the clearing pass after running the V cut.

Thanks for all of the responses,
Marcus

[ElevationCreations]

We have had issues with the angle on the Whiteside bits, some are right on 60 degrees, others are plus or minus. Judging from the photos and my experience it looks like the angle is off.

Keep in mind if you have your start depth at .2" and flat depth at +.1, your total DOC on the tool path is .3", which the v bit will attempt to cut in one pass with the Max DOC setting at .2" since the tool path will think that the DOC is only .1" which is < .2". I hope this makes sense.

[coopcnc]

That's disappointing about Whiteside, I was under the impression they were the good bits. On the passes I do .2 DOC on the Recess and for the plug it's .1 start depth and .1 DOC so no more than .2 for each.

Thanks for the time looking into it, I'll try another bit and see what happens.
Marcus

[gkas]

Try reading this thread. I think it will be a big help.

Checking V Bit Angles http://forum.vectric.com/viewtopic.php? ... vbit+angle

[coopcnc]

So I switched to a 45 degree V Bit and ran the tool paths again. Belts are all tight, but exactly the same result????

[adze_cnc]

Can't read Aspire file but here is an observation and a question to investigate:

The inner bowl of the R in MDF is quite smooth. But it is also smooth in the "preview" image. Notice that the edges of the R that are ragged in MDF are also ragged in the "preview". Why is the one smooth and the others are not?

Steven

[coopcnc]

Good question, however the inside edge of the slant on the main part of the R is smooth on the simulation but jagged on the cut. Again, it seems to be affected by adjacent cuts that approach the side of the letter and thus cause the bit to raise to clear them. I may be asking too much of the software or machine to account for this, but others don't seem to have an issue so it must be me somehow.

[laflippin]

Not sure what your problem arises from, but concerns over the exact angle integrity of the bit do not make sense to me if you are using exactly the same V-bit for carving both the female and the male workpieces for your Zank inlay project.

[ElevationCreations]

It will take some time to understand the limits of your machine and how to work around them. We have been running Shapeoko 3's since they were introduced and have 3, two with the HDZ upgrade. Our our first machine serial number was 0063.

Regarding the V-Bit Angles, each manufacturer can have variances, the correct angle is critical on V-Inlays as any error will double once you place the male inlay in the female pocket.

• Tram your waste board
• Try measuring your V Bit angle to ensure it is 60 degrees. If not, then adjust your settings in the software to what you measure the angle.
• Adjust your max DOC on your V Bit to .05" - This will allow a not so aggressive final cut (it will take two passes from the starting depth to the flat depth)
• Slow your feed rate on the final pass of the V - Bit
• Create a pocketing operation to clear waste from the V-Bit area from the material surface to the starting depth to minimize how much material the V Bit has to remove on the first pass of the tool path

Another method you can try is to duplicate the V-Carve tool path and adjust your settings to make a roughing pass with the V-Bit not as shallow and a finish pass by running both V-Bit Tool Paths

• Example:
  If you wish for a total depth of cut of .3", and your final Start Depth is .2" and flat depth of .1" resulting in .3" Total depth of cut for the mail inlay
• Inlay V-Carve TP 1 - Start Depth .17" Flat Depth .1" - Will Cut shallower than the desired finish by .03"
• Inlay V-Carve TP 2 - Start Depth .2" Flat Depth .1" - Will cut to desired profile, will only require removing .03" of material resulting in less deflection on the bit. Recommend a reduced feed rate. The max DOC for this tool should be greater than the flat depth so that you only have one pass on the V-Bit.

Hope this helps, the machine can do what you are asking of it. It won't make cuts like a machine that has linear guides, a steel frame, and 3HP spindle.

[laflippin]

Re: "Regarding the V-Bit Angles, each manufacturer can have variances, the correct angle is critical on V-Inlays as any error will double once you place the male inlay in the female pocket."

I'm not sure that I follow that logic. If a 60 degree V-bit is used to make the female engraving for a Zank inlay project, and the same V-bit is used to carve the male (mirror image) piece, the slopes of the walls of the female engraving will exactly match the corresponding slopes in the male piece. So, if your V-bit is actually 52 degrees instead of 60, but you are careful to use the same bit for both parts of your project, the slope of the V-shaped grooves in the female engraving will still match up with the corresponding edge-angles of your male workpiece because the female and male pieces are mirror images of one another.

Am I missing something?