I am attempting my first “big” (about 10X10in) inlay for a large maple brisket board with the inlay being walnut. anyways, the design was provided by the person. Threw it into VCarve Pro and made some minor tweaks. Went to do a test cut to see how my parameters turn out. Both v carves seem extremely long. Female cut is 4+ hrs and male is 8+ hours with a DOC of only .25in. Using standard DC EMs to do the clearing and a 30* V. I have watched every YT video under the sun it feels like, regarding inlays. Even smaller and “simpler” inlays like a name for instance, seem to be way to long on the cuts. Is there any insight or advice anyone could throw my way? I’m trying to understand but I just don’t think it is clicking for me. Thank you.
There is often no need to clear the entire male/plug side. If you have a bandsaw, you can just add a small offset around the plug and cut it out. Or you could probably use the CNC to make a profile cut.
Can you post the VCarve files or at least a picture of what you are working with? If the file types aren’t supported in the forum, you can upload them to the Dropbox link here:
I put the V Carve file in the Dropbox. Let me know if there are any issues with the upload.
Thank you for taking a look at them.
I’m not sure if you are on a different version of VCarve, but it is complaining a little. Still, I can give some basic feedback. Your biggest time issues are arising from the 30° bit settings.
The pass depth for the 30° bit is really low. It will require a lot of passes to achieve any notable depth, which will add a lot of time. I would expect a pass depth closer to 0.125", but I am not familiar with this particular bit.
The feed rate also seems low, but it does appear to be within the range of what the website at that link says.
The clearance pass stepover (and final pass stepover) could be increased to 100% since this is an inlay. Any cleared areas on the female/socket side will be hidden beneath the inlay and the cleared areas on the male/plug side will be cut away. There is supposed to be a small gap at the bottom of the inlay anyhow, and a rough surface is good for the glue-up.
I am assuming the spindle speed is irrelevant and you are manually adjusting the router?
Additionally, here is an example of what I was referring to with the plug side. You could save some time by just cutting the part out instead of clearing the whole exterior.
Instead of this:
I’m working with VCarve Pro version 11.014. But this is all making sense. However, all of the speeds and feeds are directly from the suppler.
In that regard, I feel like increasing any of parameters would be too excessive for that particular bit? I could be wrong though.
The profile cut is a great idea, as I don’t have a bandsaw just yet.
Basically, what it all boils down to is the pass depth is really low and that is what is where the time stacks up. So, either bump up the speeds and feeds or find a bit that knowingly can handle what we are asking of it?
If that’s all that bit can handle, then it’s just going to have to make a lot of passes. But you can still increase both the clearance pass stepover and final pass stepover to 100% to speed up the carve significantly. The quality of those clearance patches is irrelevant for an inlay, so it’s currently overkill.
After reading more about it, that actually sounds like a really interesting bit. But some of the specs on the webpage are different than the table you posted above, so I’m not sure what to think. Makes me wonder if the DOC is a typo.
I increased the clearance and final pass stepover and that decreased the time significantly.
and the future is now, I ordered the 45771-K. lol
One more confusion I am having. For the inlay cut. Do you recommend that I create one individual V Carve tool path going to the depth I need, or should I step it down like I did in the file that I sent you, with the Start Depth increasing with every tool path created? I have read doing it both ways. Is that a “more than one way to skin a cat” kind of deal?
interesting. It came in a bit set I purchased. I didn’t think to look into the bit individually.
Yes, if you are going to work at a “start depth,” as you will need to do for the plug side, you should step down incrementally. Otherwise, you will plunge straight into the material to your defined pass depth plus the start depth. You would need to go to the start depth of the next pass, and so on.
Thank you for your help and insight. It is much appreciated. I am going to apply all this when I get the bit in. Thanks again and I will let you know how it all turns out. good or bad.
Sounds good. I look forward to seeing it!
If it’s one of Garrett’s (IDC Woodcraft) it’s likely a typo. I found a few when I was looking at his charts & gave him the Makita speed vs dial chart so he could add the dial settings. He also initially set those up for a really weak machine and even though he’s using a better one now, I don’t think he’s updated all of the settings. I use chip loads to calculate my speeds so I haven’t done much with charts like this because unfortunately they lack the chipload factor.
It is from IDC. Have you been able to come across the chip loads? I haven’t been able to find them for the bits.
He doesn’t provide that info which is one reason I don’t use his bits. He’s oriented more toward the casual “plug & play” user where chip loads are too confusing. So his speeds tend to be very conservative for a 1F setup.
I recently started doing some vcarve inlays also, and my test pieces have about the same level of detail as yours. I am using a 60deg bit and it seems to get all the detail I need altho I do get some chip out on the male maple piece. I think a good quality 60 deg bit can get you there a lot quicker. Just my .02. I have a 30 and 60 on order that this guy uses Vcarve Inlay Coasters. Here is a pic of 2 test pieces using my Whiteside 60 1502 V Groove, which I think is not a great vcarve bit.
Those look great! Undoubtedly, a 60° bit will make a beautiful inlay.
Still, it may be worth considering the use case when deciding which bit to use. For example, a deeper carve/inlay may be beneficial for the longevity of a product such as a cutting board where chip-out may be a concern. A deeper inlay also means more surface area for a stronger glue-up.
It can be helpful to visualize just how quickly the depth of cut increases with a smaller bit angle:
After a number of trials and failures carving fine detailed inlays, my solution was using the Amana 45611-K, which is a 15 degree having .005 tip and is pretty amazing in my opinion, along with a tiny 1.8mm (~5/64) cheap corn cobb end mill intended for the laptop 3018 CNC machines as a clearing bit. The settings I use include: Female = Start - 0, Flat depth. - 0.1575" and Male Start and flat depths are both .0787" (female flat depth divided by 2).
Also, my carving times for a pretty large inlay are about 2 hours for the female and about 2.5 hours for the male.
Lastly, one suggestion I can make is to carve using the V-bit FIRST, then the clearing bit. Doing this helps prevent blowout of the fine lines as there’s material on both sides for the V-bit to cut through.
I’m also struggeling with vey detailed inlay… what a challenge !!
I aslo use with a 15 deg 0.5 tip and using 5 up to 7mm depth for the pocket
I’ll test by starting with the V-bit instead of the clearance, thx for this share
Even with this bit, very thin lines are posing problems, I m searching a way to find all lines < 1mm with Aspire before to carve.
This will help to detect critical areas, adapt and finally avoid failures
Did you found a way for a preliminary test strategy like this ?
I’m using Aspire pro 11 and get access to tools like : illustrator + photoshop + inkscape
Some ideas ??