Small radius inlay

[magazines]

Hello All,
Thanks in advance for any assistance you can provide. We are trying to work with inlay now after primarily using our machine for straight independent cuts for a number of years.
We set up to cut a test and the first one went great. Same bit for each male and female, no last pass to get into the corners as usual.
I should say that our common practice is to run a cut with, say, a 1/4" end mill around the shape and then follow in the corner radii to clean with an 1/8 or 1/16th - just cutting air except in the internal corners. I had always wondered why there wasn't a shortcut for a final pass in the internal corners and now I am even more curious. We are an academic setting and speed is not as much of a pressing issue as a true production shop, so we know we have a bit of a different situation than a lot of folks.

So, we set up to cut our test a second time and used the normal 1/4", cut the male and female and then returned to chase the bits out of the internal corners with an 1/8" to get a sharper look. Well, you know what we got, I bet. I've included photos below to clarify, but the automated inlay system cut the expected radius into the female hole and did the same on the outside pointed parts of the male part. The inverted parts are fine- where it digs into the corner. Kinda figured that might happen, but now I'm trying to see how people work around smaller radius bits.

I googled and looked on this forum and the shopbot one (we have 4x8 spindle version) but couldn't figure it out. Since it seems so easy to get higher resolution, finer cuts by running a final pass with a small bit, I'd think this was even more emphasized on inlay. Do people run a male then female profile and then a last pass inlay on each with smaller bit? Or some other workaround? It seems ripe for an option to just click, but maybe I'm just being dense here.
We are also experimenting with the vcarve method, but really need to make interlocking full depth pieces. We do understand that is standard for high-definition surface inlay.
Thanks!
Peter

overview with indications

detail of female

[potzmannwoodshop]

The only way i know of to get sharp corners in an inlay is to use the vcarve technique, other than that you are stuck with the radius of your smallest cutter as the tightest "point" you can form.

[mtylerfl]

I suggest reviewing the video tutorial on the software male/female cutting of inlay parts. Done correctly, you won't have the radii voids like you show in your photo.

To eliminate "round corners" altogether, you can use the VCarve inlay technique (but they won't be "thru" inlays that have the same appearance from either side, if that's what you're after). Lots of good info in the VCarve inlay thread if you need details on that method.


Hmmm. Went to the Vectric Training site and didn't spot a male/female inlay video tutorial. Did a quick google and found this one on youtube. It has all the pertinent info:

[magazines]

Thanks for the replies.
We do need the full depth male female or we would go with the surface inlay method with the Vcarve though.
Our first effort was a 1/4" and followed the video that you linked, mtylerfl. It worked fantastic, but does leave the standard radius.
That's totally understandable, but we pretty much always run the last pass on detailed work with a smaller bit to get rid of the little bits of radius in corners. I guess I thought this was quite common - though it does mean cutting quite a bit of air. But last pass is something that is included as a option in the software. And we did try to run some jobs with just 1/8 or 1/16 all the way through, but you can imagine that we killed a bunch of bits before we figured out the last pass with smaller radius trick.

So, is there no workaround for the inlay with smaller bit that anyone knows of?
Thanks for looking!
Peter

[mtylerfl]

Hi Peter,

Not really a workaround, but "standard practice"...for best results and good fit every time, just use your smallest radius bit throughout the entire process. This achieves your goal on minimizing the radius at the corners and yields an acceptable outcome.

If you were breaking bits, then it's probably a feed and pass depth issue that needs to be addressed and corrected.

[magazines]

Hello Myterfl,

Ok, we will experiment with ways to pre-cut before the official inlay run to see if we can get this to work. Or maybe redraw the vector with bump outs for the needed spaces of curvature. Still trying to think about this. And we see this as a very useful feature request for a last pass with smaller bit - for general profile/pocket cuts, but especially in this case with inlay.

Just to clarify, we didn't break a bunch of bits, maybe just one or two. But we did realize if we are setting up for a big 4x8' intricate cut, we were going to have better tooling life if we ran it first with 1/4 or 3/8 bit an then go down to 1/8" or 1/16" to get the finer details. Even from the beginning this seemed like good "standard practice" as we understood it - for cutting speed, reduce deflection, and yes, to avoid breaking bits. Would you go at a big, detailed job with a 1/16" bit first?
Thanks,
Peter

[mtylerfl]

Use the same bit through the entire project. Do not attempt to swap bits. Both male and female parts must have the same bit so that the inside and outside radii match up.

Big projects like a 4'x8' will look fine with a 1/8" radius in the corners (using a 1/4" end mill for all cutting of male and female parts).

Reserve the use of 1/8" and smaller end mills for small projects of course.

[magazines]

Hi Michael,
Now I'm a little confused. We run projects all the time that have multiple different bits for them - an end mill for the profile, a ballnose for a pocket, a vcarve for engraving or carving. Is that unusual in Vectric practice? And as stated, we usually want more detail on projects than a final pass with a 1/4" end mill can provide.
As we mentioned, we do recognize that the normal usage of the inlay through cut is to use the same bit, for the reason of making sure that the male-female radii match up. But we almost always run a last pass for other projects with a smaller bit such as a 1/16" or 1/8" to get a finer quality, higher resolution image. I think that we have confirmed that this may be unusual in the community, but we have definitely seen fabricators with MasterCam and other systems doing the same, so it's not industry unusual. We just wanted to see if there was a way to do something that seems somewhat normal in the industry with the inlay tool of vcarve/aspire. Due to the nature of the (excellent) inlay procedure in vcarve, we notice the radius significantly more and consequently experimented with our normal method. Finding this not to work, we decided to ask the forum.
But it does seem unusual to approach each CNC job with a single bit if that is what is advised.
If our experiments develop any success we will post the results and methods here for others.
ok, thanks,
Peter

[mtylerfl]

Hi Peter,

I believe you are confusing other types of cutting processes vs the Inlay procedure. But, be that as it may, at least you're challenging yourselves and hopefully learning some things in the process.

[Adrian]

I use multiple bits all the times in jobs as do many other regular users here. Personally I would do it by creating the correct vectors and use the profile toolpath. Double inset/offset with the bit radius will yield the correct vectors.

[mtylerfl]

I use multiple bits all the times in jobs as do many other regular users here. Personally I would do it by creating the correct vectors and use the profile toolpath. Double inset/offset with the bit radius will yield the correct vectors.

Yes, that manual method is essentially the same way the Inlay male/female inlay feature works - but it's automatic. (I've used the manual method myself, BTW.)

Still won't solve Peter's "problem" of trying to reduce the cutting radius plus achieve a tight male/female fit without gaps in corners when including a bit with a larger radius in the mix!

The "manual" method as well as the "auto" method both require the same bit radius consideration between male/female parts to fit together.

[Adrian]

I must be misunderstanding the issue then. I would cut with the 1/4" bit and then cut again with the smaller bit but only using the parts of the vectors that would yield the removal of more material. That's why I would manually create the vectors rather than using the inlay toolpath.

[mtylerfl]

Perhaps (if you have time), you can post an example file.

You may be thinking along the line I did, by having multiple sets of vectors. Essentially profile cutting up to areas of inside corners, with say a .25" dia. EM, then stopping the cut before it would remove material in a corner of say a .0625" radius (a .125" dia. EM). Then, using a subset of vectors only for the small inside corners, do final cutting with a .125" dia. EM.

Not impossible, but could be a heck of a lot of work depending upon the item(s) being inlaid this way.

For example, a simple five-point star wouldn't be too bad or time-consuming to create separate vectors for the inside corners. But a more complex item such as a palm frond with a "zillion" inside corners might be more pain than what it's worth to create separate inside corner vector paths for the smaller bit.

Not sure if I'm communicating this well or not, but I hope it's understood! Another possible bugaboo using two different Bit diameters to form a complete cut in two operations is whether witness marks and/or Bit runout would interfere with the final fitting.

[mtylerfl]

Can't help chuckling to myself a little... Sitting here thinking how funny it is to make a normally simple male/female inlay process complicated!

[magazines]

Hello All,
Just posting to confirm the method to do this. Thanks for all of the suggestions. In the end I guess it was pretty straightforward.

We got it to work with an outside profile cut on the male piece and an inside profile cut on the female piece with the 1/4" bit and then follow up with a normal straight inlay male and female both with the 1/16" bit.

So more work, but not too much more complicated than an ordinary last pass for a higher resolution result. I guess the one thing I'd say is that if we can have a last pass for smooth finish or to facilitate part removal, why can't we have a last pass for cutting only the corners, for inlay, profile or pocket?
Thanks,
Peter