Square corner trick

[nick]

I need to rout a box inside a raised panel door with a 120 deg V bit. The inside corners are square but the outside corners have a radius from the diameter of the tool. What is the trick to squaring the inside and outside of the V groove.
Thanks

[signtist]

You need Aspire software.

[billp]

Nick,
Here's one way to do the insides...I'm sure others will have their solutions as well.
7714
The bit is from MSC ( www.mscdirect.com (http://www.mscdirect.com))#01855188

[myxpykalix]

bill what is the diameter at the tip of the bit and couldn't you use say a 1/8th" endmill? What is the advantage to using this bit?

[billp]

Jack,
http://www1.mscdirect.com/CGI/IMLMKD
The advantage is that it's tip is small.....

[nick]

Thanks Guys...I have Aspire but was looking for a way to lift the cutter in the corners to square the outside edge. This way would be much easier then 3D machining the corner.

[bleeth]

Nick: Freedoors does this. Do a quick search on the forum. It is a free program. It is designed to do typical mdf doors resembling the thermoformed ones. It will require bit changes.
Disclaimer: Never used it myself so I don't know the limitations design-wise but lots of botters have.

[john_l]

Nick. In Aspire... Click "Create Profile Toolpath", select your V bit, set cut depth, down in the middle.. click corners tab and check both "sharp internal" and "sharp external".

Is that what you mean? Hope this helps.

[jdervin]

If you don't mind using something other than your ShopBot, these corner chisels could do the trick:

http://woodworker.com/corner-chisel-mssu-107-999.asp

[adrianm]

I do it the way John L describes all the time and it works great.

You don't even need Aspire, Partworks has the same feature.

[joe]

http://www.precisebits.com/products/carbidebits/taperedcarve250b4f.asp

$29.00

[jdervin]

Bill,

In the photo example you provided above, I'm not exactly sure how you would use that bit. I'm guessing that you first do an area clearance with a larger end-mill, and then do an inside profile with the bit you've shown, but if so, I would think there would be some leftover material between the fillet left behind by the end-mill and the tight corner cut by the 1/32" tip of the tapered end-mill.

Would you be so kind as to describe the toolpaths (and any other steps) you used?

[billp]

John,
Before some of the current software solutions were in place the easiest trick was to do exactly as you stated, run an inside profile with a small bit after making a pass (or two) with a larger bit to clear an area. Then it was simply a quick pass with a sharp chisel, and you'd be done.If there was a fillet left you'd just go back and machine that out, although some people just used the chisel for this as well. The smaller the bit, the less to remove.....
PS- Those people who had software which featured "rest machining" also let the program go back and take care of this in a separate pass. Rest machining "knows"which areas your first bit didn't get to ( the fillet) and then ONLY goes back and clears that out. I believe that is now in many software packages.

[jay_d_wyant]

Nick,

I am not sure I understand your question, but if I did, then I don't think anyone else did.

If you are using a V-bit and want square inside and out side corners on a V-Groove, then use a V-Carving toolpath.

At least that seems like what you are asking.

[jay_d_wyant]

And by the way, you would need to draw and select two vectors representing the inside and outside of the groove.

[Gary Campbell]

Nick...
Do you mean corners like this:

7715

These were done as an inside profile using a V bit with inside and outside sharp corners selected.

Use these Settings adjusted to your bit & machine:


7716

Gary

[richards]

It's a very simple process if you're willing to insert a little handwritten code into your program. Do a little trig to find the ratio between the depth of cut and the angle of the cutter. A 90-degree cutter is 1:1, a 120-degree cutter is 1.72:1. (I cheated and drew the cut in AutoCAD LT and then used the dimensioning tools to give me the numbers - just so that I didn't have to admit that I can never remember whether to use Sine, Tangent or Cosine on a calculator.)

Since you know the depth of the cut, multiply that number by the ratio. Enter a command in your file to change from absolute mode to relative mode (SR). Do a 3-D move the distance of the number that you just computed in the desired direction.

Example:

Your cut is 0.25 deep.
You're using a 120-degree cutter. (The angle of each side is 60-degrees from the centerline of the cutter.)
The ratio is 1.72:1
You want to move the cut towards the 0,0 corner of the part.

Length of cut = 1.72 X 0.25 = 0.43"

Code snippet:

SR
M3, -0.43, -0.43, 0.25
M3, 0.43, 0.43, -0.25
SA

That piece of code moves both the X-axis and the Y-axis the proper distance as the Z-axis is lifted. Then the process is reversed to put the cutter back to the original position. Just change the sign (+/-) depending on which way you need to move the cutter.

If your cut is on an angle, you'll have to break out the calculator and use a little more trig to calculate the ratio between the X-axis and the Y-axis. If you're going to do a lot of corner cutting, you can look at the source code for the doors.exe program in FreeDoors - the program that Bruce Clark and I wrote. The C++ formulas are there that show how I compute the 'sharpening' moves for any angle."