Inlay Pocket Clearing Problem

[dbrook]

I watched Andy Johnson's inlay video from the virtual user group meeting and have followed his guidelines to the letter in making an inlay that is approximately 5" x 6" in walnut. After three attempts at cutting a clean female pocket I have run out of options and need the benefit of some thinking of the experts on the forum.

When you check out the attached pictures you will see where the flat area at the bottom of the pocket never gets cleaned off flat in the corners. On my first attempt I used a 0.125" spiral up cut end mill for the clearance cut followed by a 1/2" 60 degree V bit. This attempt resulted in a small uncleared area in each of the corners . This first attempt was cut on my my 4 ft x 5 ft rack and pinion based router. I thought the problem might be a result of the backlash in the system so I tried my second attempt on my small router that is driven with ball screws and is more accurate using the same bits. This attempt again resulted in the same uncleared areas in the corners. On my third attempt which I cut on the ball screw based router I used a 0.125" spiral up cut end mill and an 0.0625 up cut end mill for the clearance cuts followed by a 1/2" 60 degree V bit. This attempt again resulted in the small raised areas in the corners but more of the raised area was removed. I next tired using only the 60 degree V bit to re-cut the entire pocket.

I have watched Todd's and Mark Lindsey's inlay video as well as others on You Tube but for the life of me I cannot figure out what I am doing wrong. The design was done in Aspire 11 and I accurately measured each of the bits. The 1/8" bit measured 0.125", the 1/16" measured 0.0625" and the V bit measured 60 degrees.

Any suggestions or thoughts on how to solve this issue would be most appreciated.

Dan

[adze_cnc]

My first thought: what are the stepover values for the square-end bits? If they are greater than 50% make them less than 50%

[ohiolyons]

Would help if you post the file.

[dbrook]

Thank you for the feedback. The step over on the 0.125 end mill was set at 80% so I cut it back to 40% as suggested. I generated the new G code and make another run in a fresh piece of wood. Unfortunately, the raised areas in the corners are still there. The .crv file is attached and I hope that someone can determine what is causing the raised areas in the corners of the pocket. After watching more online videos and seeing the success that other people are having doing inlays I must be overlooking something or doing something wrong. Any additional input would be most appreciated.

Dan

[adze_cnc]

I don't have Aspire so I can't look at your file.

The following may be instructive:
 

 
90 degree v-bit parameters:

• Final Pass Stepover: 0.0562 inches (7.5%)
• Clearance Pass Stepover: 0.1125 inches (15%)

 

 
90 degree v-bit parameters:

• Final Pass Stepover: 0.01 inches (1.3%)
• Clearance Pass Stepover: 0.1125 inches (15%)

[ohiolyons]

You must use a smaller bit.

Just watching videos where someone's design worked doesn't mean you aren't doing it the way they did.

I know a person who just loves this swirly scripted looking Germanic font and complains that small pieces are constantly breaking off.

What people don't understand is that there are some designs/fonts that don't inlay well.
Even worse when small in size.

Why are you worrying about the part that is going to be covered by the male inlay?
Knock it off with a chisel.
Sometimes a CNC isn't the best tool for job.

[adze_cnc]

It matters if the height of the "nub" is taller than the "glue gap" and there are a great number of corners with ones where a chisel wont fit.

As my images show I suspect the OP just needs to look at the v-bit's stepover parameters. Sometimes setting big stepovers to clear out more material at a time can cause more hassles than they are worth.

[martin54]

Have a good look at the toolpath preview to see if those uncut parts show in the preview, as well as checking the stepover as adze_cnc has suggested you may also want to make sure a 60 degree bit fits all the way to the bottom of your angled corners.
Not got software installed on this machine so can't check the file

[Adrian]

I think there is something else going on here other than stepover. The islands left at the top left and right of the triangle in the photo, for example, don't correspond with areas that the v-bit machines. The bottom does but the nub is nowhere near as big as the picture.

There are quite pronounced ridges between the passes on the edge of the cut and a quite few areas that should be going to a sharp point but are rounded instead.

I would be checking the usual things with odd v-carve results such v-bit angles, feed rates and free play/binding in the machine. I've no idea of the capabilities of the machine but I know of some that would really struggle to cut hardwood at those speeds.

[Adrian]

Looking at it in a bit more detail those islands correspond with the areas that the "V-Carve 1 [Clear 2]" toolpath should be cutting. It almost looks as though that toolpath hasn't been run at all. Personally I would just delete that tool entirely and recalculate as it's not really needed. Just run with the 1/8" tool and the v-bit.

There's still something not right with the v-bit part of the job though as a lot of the corners aren't sharp.

[adze_cnc]

It's interesting that some of the corners are OK while others are not. You can really see it in the "negative" of the original image:
 

 
The corner in the lower left looks good. The line where two planes meet comes to the top of the material. For the corner in the lower right you can see where that plane line comes to a stop and the corner is rounded.

[dbrook]

Thank each of you for your feedback. I really appreciate you taking your time to help. Clearly, there are several things I need to investigate in the software settings and on the machine.

Dan

[Jan.vanderlinden]

The first thing that popped into my pea brain.
Is your machine tramed in?
Is your material flat?

[dbrook]

Thank you Jan for the additional suggestion. Yes, the spindle had been trammed and I made sure the material was flat as well as of a uniform thickness. Fortunately, after checking my settings in the software and making the suggested changes I was successful in creating a good inlay. Final settings that worked are as follows.

1 . Reduced the feed rate from 100 ipm to 50 ipm and reduced the stepover to 20% for the 1/8" spiral up cut mill used for the clearance tool path.
2. Set the Clearance Pass Stepover to 15% and the Final Pass Stepover to 7.5% for the 60 degree V bit.
3. Clamped the board to the spoil board more securely with stronger hold down clamps.

Thanks again for all the good suggestions and ideas.

Happy holidays to you all.

Dan

[FixitMike]

I would like to point out that the "stepover" percentage for a V-bit is misleading. It is calculated from the largest diameter of the bit, but doesn't reflect how the bit will cut the surface. The linear measurement (inches or mm) is what affects what the surface will be.
.01 inches stepover for different diameters of V-bits (with the same included angle) will have different percentages, but the cut will be the same.