Gaps in inlays?

[tyger_purr]

Is this what I should expect?

My inlays have gaps. Is this because i was using cheap wood?

[drueth]

tiger_purr

It looks like a problem with the gantry flexing. This could be because of the speed of your cut or the bit not being sharp and causing to much drag, and causing the bit to move in and out of the true tool path.
I know of three different way to do and inlay and I have had problems like this with all three. What I have found is EVERTHING must be dead on for an inlay to come out right.
It looks like you used the inlay tool path option. This can also be done using Vcarve / Engraving method and also a modified version using the Vcarve for the female pocket and the Prism carve for the male insert.
So my question is which shark do you have, Which method are you using to do the inlay, How fast are you going.

And one that can cause lots of problems. Have you done a test cut to find the TRUE angle/dia of the bit you are using.

[tyger_purr]

I am using a piranha with a Bosch Colt. I've only had it for a couple of months.
I am using VCarve desktop 8.020 Inlay (male and female) tool path
I am using a 1/8" end mill at feed rate 60 inches/min. I believe the router is set to it's highest speed which the literature claims is 35,000 rpm. 20 ipm plunge.
It is set to cut a 1/4" deep pocket in 3 passes (0.0833 per pass).

The prototype is made from big box store cheap white wood with poplar inlays.
The final product will be walnut and maple. I was going to cut the feed rated down (probably 30ipm) before I ran these.

I am new at this so I am open to any and all advise.

[Eagle55]

I think I would tend to agree with drueth. Feed rate sound like it might be a little marginal and flex is always looming in the wings. With it being really close, but not perfect, I would certainly try cutting the feed in half via the FRO slider and see if it takes you in a good direction. And maybe even reduce the pass depth a little to. After all you are just looking for a small amount of improvement.

Roger

[drueth]

tiger_purr

Lower the speed on the router down to about 12K rpm. I would set the Pass depth to 1/2 of the diam. of the bit or 0.062. Also the step over need to be only about 10%. ( This will cause your run time to go up and can be delt with by using a second bit and do a "large area clearance tool path also ) This should lower the load on the bit and prevent the flexing that most all sharks have. With the router off, See how much you can move the tip of the bit with your finger in the X and Y direction. This is the issue you need to deal with and overcome so the cut come out better.
The wood is not the issue causing the gap you see. It is most probably the router flexing/moving/tilting in it mount ( just what you saw when you used your finger and pressed on the bit ( it moves)) . You would never see this problem with almost any other cut you can do with the shark.
I would also do a test cut with the end mill you are using and measure the cut very carefully. Lay out 2 squares one inside the other let say a 2" outer square with a 1" inside of the 2" The depth of cut need to only be about .125" . Use a pocket tool path to cut out the area between the two squares. Cut an measure them. My best guess it the 2" will measure about 1.95 - 1.98" and the 1" will measure about 1.02 - 1.05". This is because most bit you buy are under sized by a small amount, and again nothing you would notice or care about with the many other thing you can do with the shark. (this "problem" can be corrected by setting the Geomerty/diameter of the bit in tool data base for the bit you are using. )

[tyger_purr]

The colt only goes down to 16,000 rpm.
I'll give that a try.