Using "Advanced VCarve" in Carbide Create 461 to make Inlays

@sjj47

4 Likes

I have tried this now a couple of times and each time everything was great except when I cut into it I noticed my inlays are like 1/8" which is fine unless you are doing a cutting board like I’ve been trying for and that doesn’t cut it. So if I need to fill a .25 pocket then my plug needs to start at .2 and a max depth of .3? this would give me a glue gap of .05" and a .05" saw gap correct? So is my problem the fact that my inlay just may not have been deep enough for a cutting board? Does anyone else think I should have done a 1/2" pocket or deeper? new to this so any thoughts or help or expertise would be welcomed. Would be great if CC just did it for you more like I hear Vectric does. Also using Advanced Vcarve for these.

I think this tutorial has been posted to these forums previously, but I can’t find it again, so check this out:

I had to watch it more than a couple of times, but the results are certainly worth it! Perhaps it’ll be of help to you as well.

2 Likes

I’m currently using Carbide Create (Build 648) and have had mixed results with this so far. Using Advanced VCarve, I’m using a 1/8" flat endmill for my area pocket tool and an Amana 46280 6.2 degree vbit for the vcarve operation.

My female pocket depth is 0.20" and for my male plug, I’ve used a 0.17 start depth and 0.20 max depth. That left me with no gap at the bottom or at the top and approximately 0.031 gap on each side of the inlay. I changed the max depth to 0.22 and that provided a gap at the top, but it was still flat against the bottom and the same 0.031" gap on each side. I changed the start depth to 0.00" and the max depth to 0.22 and that decreased the gap on each side to approximately 0.015". Close, but not quite there and still no gap at the bottom. I finally scaled the model up by a factor of 1.034 and that got me a perfect fit. However, I don’t see scaling the model as the best solution.

What am I missing? Is there something I’m not considering with the vbit I am using? Other offset adjustments I should make? Thanks for any advice you might have…

You should be okay with your first settings if you make the max depth deeper by at least .031” It seems like you need to push deeper with your settings.
If you watch the video posted just above your reply, it gives some very detailed explanations for why this is necessary.
You are also making it harder on yourself with the 6 degree v bit. Watch that video from minute 2:00 to about 3:30 for an explanation about why you need an angle for the inlay to work right. It is easier if you use a wider angle bit.

You dont need to go deeper on the female part (.2") but start depth needs be .1" on male plug.

Check out my post near the bottom.

You’re using a tapered ball mill, not a v-bit.
You’re Z-zero is too low and your angle is likely incorrect. The true point of a 6.2deg V-bit would be over 3mm below the end of the radius on the bit you’re using. The software you’re using has does not know the exact geometry of your endmill…it assumes a true point. Use a v-bit or adjust your Z-zero up 1/8" or so. Even then, it won’t be quite right because of the tip radius, but that is probably not big enough to cause much issue as long as you account for the Z-offset.
Tapered ball mill angles are assigned differently as well. If it was a V-bit, it would be a 12.4deg. That’s another MAJOR issue depending on how you set that up. If you have it set as a 6.2deg v-bit, you’re cutting twice as wide. Combine that with cutting too deep and you’ll never get a good fit.
Basically, a tapered ball mill is not a V-bit and isn’t a good choice for prismatic V-inlays.

Your 6.2deg tapered ball overlaid on what would be a 12.4deg V-bit.

3 Likes

I had very similar struggles with mixed results as you experienced. Followed many of the steps I think you attempted by changing the mixture of pocket, start and max depth, as well as scaling up in the inlay or creating offsets. Another poster pointed out what I think has already been added to this thread in regards to narrow tapered ball mill relative to a true v-bit. In the end made the decision to add Vcarve Desktop which I think has more functionality to account for the geometry of a bit like Amana 46280. Using that software, was able to successfully make a somewhat fine detailed inlay 0.25 into a walnut end grain cutting board using the exact Amana 46280 you described with no extra adjustments necessary.

11 Likes

Thanks Neil. Great explanation on the tapered ball vs. the vbit. The differences may seem insignificant, but in reality, the extra 3mm of length are huge when doing this level of detailed work. I did attempt to adjust the settings based on these new principles, but still couldn’t get exactly the results I was looking for. I ended up switching to a Whiteside 22 degree vbit (#SC50) and got the results I wanted on the first try.

1 Like

Thanks Todd for validating my experience with this bit. Carbide Create does some things really well, but clearly has its limitations. I’ve switched most of my design and machining over to Fusion 360 (free) and only use Carbide Create for quick and simple operations. Eventually, I may switch over to VCarve Desktop, but I still choke on the price for now. Fantastic results on that cutting board by the way…

thank you! The walnut board was going to be for us, but got repurposed as a gift to a friend with the flower inlay–haven’t had time to get back to the shop to make our board yet, but have all the tool paths tested out already. I toyed with the Whiteside SC50 a little bit as well in Carbide Create and seemed to conclude it works for inlays so long as the inlay is of a minimum width at the surface. For thin widths and/or fine details closely spaced, I feel that the narrower angle of something like the 6.2 degree tapered ball mill is needed.

This topic was automatically closed after 14 days. New replies are no longer allowed.

This is all great info; and glad to see the discussion open back up.

The thing I’m getting hung up on currently is when cutting the male part. If the start depth on an advanced vcarve on male part is .1", the 1/8" flat end mill seems to struggle, and I’m afraid the bit will break. This is in pine, so prob fine, but I’m planning on moving to harder woods. Is it only me that worries about the .1" start placing strain on the bit?

Also, it’s asking me to take the 1/8" bit pass down to 10,000 rpm, or setting 1 on the carbide spindle. Is that correct?

1 Like

actually the feedrate (speed at which the whole router moves in x/y) should be reduced as a way to compensate for the deeper-than-normal depth-of-cut…

Force goes up (sort of linear) with FeedRate, Depth of Cut (as well as having an older, more dull, bit)
Force goes down (again sort of linear) with number of flutes of the bit and higher router RPMs

what breaks the bit is high force… but you can trade these things against each other to some degree

better/more detail at THE ebook on this Introduction - Shapeoko CNC A to Z

3 Likes

That is not an unreasonable worry, especially if you’re moving up to hardwoods.

I would create 2 toolpaths, one at 0.05 deep, and the finish pass at 0.1 deep.

3 Likes

Thanks; to clarify, I had thought that having a lower spindle RPM with a deep cut would put more strain on the bit, but are you saying lower speed is better?

Carbide create is requesting the lower spindle speed on this advance vcarve, whereas I would have imagined (with my admittedly limited knowledge) that a higher RPM would reduce the lateral strain on the bit. Typical contour and pocket cuts with that bit are at 18000, or so I thought.

Thanks; I’ll try that.

1 Like

I think what fenrus was alluding to is… No, that is not correct. :wink:

For any material / tool / machine combination there is a “sweet spot” ideal SFM (Surface Feet per Minute), or linear speed at which the cutting edge of the tool travels through the material. This should not change once determined. There are many variables including material properties, tool material, lead & rake angles of the cutting edge, machine stability & horsepower, et.al. SFM is a product of RPM and Diameter, so for the same diameter you will want a similar RPM.

Safe to say for wood any 1/8" tool you use is going to be in the 20,000 - 24,000 range (or faster if the spindle will do it.) Unless you are cutting plastic, then the higher speeds will melt the material.

I don’t see any 1/8" tools in the CC library that call for 10000 RPM. The Hard Plastic single flute drops to 18000. All the other 1/8" tools are set at 24000.

4 Likes

Thanks; I’ve just checked my tool paths, and for some reason the rpm was set to 10000. I have no idea why, but have re-loaded the tool and it’s now 18000. I initially assumed that it was related to the advanced vcarve, which I’ve not really used yet.