Inlay Test For Christmas Presents

[dana_swift]

I prefer to make Christmas presents rather than buy them. Since its that time of year I have been considering several options.

Remembering an inlay technique by Paul Zank that I was told about by Bill P. I decided to give it a test. Then the presents can truely be personalized.

I read up on Pauls technique, and in just about two hours made my first test. I used a pine board for the female inlay, and a bit of "ruined" rosewood for my male reverse "outlay". (Why to keep colorful scrap!)

Here is Pauls writeup on his method:

http://www.talkshopbot.com/forum/messages/2/14775.html

It came out better than I expected. My V carve bit was a bit dull and the points of the male lettering were very fuzzy, so I did not expect a good result. Wrong! The fuzzy parts are burried deep in the female V grooves. And probably it gave more for the glue to grab.

Here is the result after using the thickness sander to remove the excess rosewood:

972

Here is the result after following up with a random orbit sander:

973

And a closeup:

974

A few quick notes: Pine earlywood is too soft for the technique to work well. I will try a 60degree bit next. This was using a 90 like Paul describes. Inlay depth was 0.100 inches, however the font made most of the inlay more like 0.050.

I have been working with Aspire to get better artwork for my next efforts. Don't want to mess up there! This will keep me out of the malls for sure.


Now I will be buying some new V bits (its about time!) And prepare to spend a long weekend making presents..

And a million thanks to Bill P.

Ho^3

D

[dlcw]

Nice job Dana.

I look forward to seeing some of the fruits of your labor in the next couple of weeks.

Don
www.diamondlakewoodworks.com (http://www.diamondlakewoodworks.com)

[porscheman]

Dana,

I just completed a large machining project for a local woodworker that involved this inlay method. I definitely got better results with a 60 degree bit than a 90 degree bit, so that's worth a try. Also, I learned from a few less-than-perfect tests that the wood used for the male portion of the inlay needs to be very dense in order to preserve all the fine details in the inlay (rather than tearing out the wood fiber).

I used the recommended depth settings in the most current version of Paul's approach (inlay pocket flat depth = .3", inlay flat depth = .2", inlay start depth = .2"). I obtained exceptional results with hard maple inlaid into walnut.

Hope this helps.

John

[dana_swift]

John- I just procured a 60 deg bit. My inlays will be more shallow, probably 0.1 or 0.2 at most. I will try some maple and see how that works for the male side.

Spent last evening creating artwork. Adjusting corners so the male female fit doesn't have fillets that wont seat.

All in all I am quite impressed with the test, it shows that my fine details are at the limit of my materials. Hard male material will make the difference. I will be keeping that in mind-

Thanks!

D

[courtney2018]

Dana, that looks really good!

[tmerrill]

Quote: Adjusting corners so the male female fit doesn't have fillets that wont seat.

Dana,

One of the advantages of this method is you don't have to make adjustments like you describe.

Tim

[dana_swift]

Tim- oh yes you do.. if the end mill wont fit into an area with inadequate clearance you get a fillet that prevents mating. The adjustment not only solves the radius problems on the end mill in the corners, it eliminates the "tight spots" that create the fillets.

Imagine trying to use a one inch end mill to make the flat areas, it could not get into most of the pocket areas to create the flat areas of either male or female causing interference. Smaller bits just have smaller interference areas, but they are still there.

Some artwork adjustment is still needed, either that or you get an interference fit. Some force required..

The technique is wonderful, but end mill size matters. One of those times when smaller is better. ;)

D

[tmerrill]

Sorry Dana,

I've never had to make an adjustment. But your sample looks great so I suggest you keep with your method.

Tim

[tmerrill]

For those interested in Paul's method I recommend you visit the Vectric forum and download Paul's excellent .pdf file with updated information.

http://www.vectric.com/forum/viewtopic.php?f=3&t=564&start=0

Tim

[harold_weber]

Dana, are you saying that it is not possible to use Paul Zank's method to do what is shown here?

975

[dana_swift]

Harold.. your star looks terrific. That does not mean it proves the problem I am speaking of does not exist.

Imagine what would have happened in the star had you used my hypothetical one inch end mill? The problem would become very clear in both the internal and external points of the star.

What happens is: in the female corners there is an area the end mill cannot reach to clear. The size of area that is not cleared is dependent on the angle of the sides in the case of the star, and the diameter of the end mill used. Same thing in the male pattern.

Now imagine lots of convex and concave detail nearby each other (within a bit-diameter), such as would happen in a photo. Now the uncleared area in the male can overlap the uncleared area in the female half, and now a real interference exists that will likely show in the final piece.

It is not always "automatically" perfect. It is normally very good, and the issue is usually hidden.

The method is wonderful, but there is something to watch out for, and artwork correction can overcome it.

I am particularly grateful for Paul's developing and sharing the method, which works "almost" perfectly.

General solution: use a small end mill and ignore the issue. Slightly better solution.. adjust the artwork for the mill size being used.

D

[harold_weber]

"Imagine what would have happened in the star had you used my hypothetical one inch end mill? The problem would become very clear in both the internal and external points of the star."

Dana - here are three screen captures first the material cut with the 1 inch diameter end mill:

976

Next, the portion cut with the 90 degree V bit:

977

Finally, a preview of both toolpaths:

978

The portion in the female inside corners that is not cleared by the end mill is cleared by the V bit when you use VCarvePro. You just check the "use flat area clearance tool" box after pressing the "create Vcarve toolpath" button. You choose the stepover for the V-bit it can be pretty coarse since no one will see the little ridges left.

OK, I've shown you how its done using a 1 inch end mill, now you show me an example that cannot be done.

[dana_swift]

Harold- As you wish- See the attachment. That is the male side with fillets left from the area clear of the 1" bit.


979

If you have a method that does not do that please inform-

D

[tmerrill]

Download, read and follow Paul's .pdf file and you will not heve this happen. That's what we are trying to tell you.

[porscheman]

Dana,

I'll chime in again here and add that I believe Harold and Tim are correct - no changes should be required to the design files to accommodate the bits that you are using for flat area clearance. That's one of the elegant aspects of Paul's approach is that you go right from a given graphic file to mating parts that fit perfectly.

I'm wondering whether you are manually creating the toolpath for the 1" clearance bit separate from the V-carve bit toolpath on the male piece. If so, that might be the problem. Instead, if you select the 1" bit as the "Flat Area Clearance Tool" in the V-carve toolpath setup, the Aspire/VCarvePro software should be intelligent enough to remove the fillets that are left behind by the 1" bit using the V-bit. Just make sure to follow Paul's suggestion in the PDF document and increase your stepover percentage from 3% to 13% so the clearing of those fillets by the V-bit is reasonably fast.

The inlay inlay work that I did had small detailed areas AND big flat areas and in no instance did I have to do any hand work to remove fillets nor make any changes to the design files provided by the client.

Regards.

John

[harold_weber]

Grr - I deleted that file I posted earlier thinking this subject would be closed closed. OK, I re-created it for you. Below is the toolpath for the V-bit cutting the male star. Notice the cleanup in the concave corners?


980

If you don't get these cleanup toolpaths and you are using Vcarve pro the only cause that comes to my mind is that you might have set your Vbit stepover to too large a number.