Suggestions for using the Auto Inlay feature in V2

[tmerrill]

I've used the new Auto Inlay feature 3 times so far and thought I'd offer a few suggestions that may help you. Some of this information is in the tutorial video and .pdf file and this is intended to complement them.

Also, this assumes the inlay is large enough where you will use the two tool option. So far, I've used a 1/8" downspiral for the small tool, and either a 1/4" or 3/8" downspiral for the large tool. Use of a downspiral is highly recommended.

First, I always cut the insert or male piece first, using an allowance offset of 0.0.

Second, cut the pocket for the female part in your material. So far I have started with a pocket allowance of 0.005".

Third, without removing the material from your machine, test fit the male piece. Be careful here, if the fit is good and you push it in too far, it can be difficult to remove (ask me how I know this...).

Last step for a perfect fit. If the fit is too tight, simply recalulate the Female Inlay Pocket, increasing the Pocket Allowance by a small amount. BUT, you only have to run the profile toolpath with your smaller tool. Only takes a few minutes to re-calculate and run and allows you to zero in on a perfect fit.

As an additional thought, you may wonder how the new Auto Inlay feature compares with Paul Z's V-Carve method. I think they complement each other and you should be able to use both methods if you want to do inlays. In my opinion, Paul's method would have the edge with detailed designs with many small pieces. For a simple design, with larger pieces, the choice is yours. For inlaying a raised 3D image that you have carved, you would have to use the Auto Inlay feature unless you can figure out a good way to turn it over and V-Carve the bottom accurately.

Hope this helps you,

Tim

[RoutnAbout]

Tim, thats a Great Tip.
Now for the real question.

How do you know?
Why shouldn't you push it in to far???
It's nice when you can sneak up on that perfect fit like that and make it work.
But don't you hate it when it sticks like that???

[Thkoutsidthebox]

Thanks for the tips.

I'd like to add that the V-Carve method would also be preferable if you need to have sharp corners instead of rounded to the tool diameter........I really have to get my new machine built!

[tmerrill]

Yes, good point. The first sample I did was a 5 point star about 4" across using a 1/16" bit. The points were surprising sharp, you had to get close to notice the radius.

Another consideration I thought of after posting is that using thin material or veneer for the inlay would require the auto inlay feature.

[NSchlee]

I've found .010" to be a good allowance amount when doing inlays, especially when gluing the parts.

Neal

[tmerrill]

Neal,

I haven't done enough to see if one value will work in all cases, but I don't think this is the case. Some factors that can affect the results include run out in your router (or spindle), actual bit diameter and bit deflection.

So far, I have had different values getting the fit I wanted.

Tim

[NSchlee]

Tim,

.010" works for approx. 90% of the wood inlays i've done.
I try to keep my machines tuned up and tight.

Neal

[tmerrill]

That's great Neal. My tip may help someone else, so I'll let it stand.

[NSchlee]

That's great Neal. My tip may help someone else, so I'll let it stand.

Tim, I'm sure it will, it's all good! Every situations different.

Neal