There have been many users who have had difficulty getting V Carved cuts to come out properly only to find that their V bits are not the angle they are advertised to be. What follows is a process to determine the bit angle of an approximately 90 degree bit by examining cuts.
The .crv file contains a triangle which has been toolpathed with bits defined as 85 through 95 degrees. Make cut files for your machine and cut a piece of scrap.
The "85" cut shows what happens when the bit angle is larger than the toolpath bit angle. Notice that the corners are bowed out a little and that the top edge looks bowed up.
The "95" cut shows what happens when the bit angle is smaller than the toolpath bit angle. Notice that the corners are bowed in a little and that the top edge looks bowed down.
I would suggest that one find the lowest number angle that looks OK and the highest number that looks OK. Average these two and that’s the angle to specify for this bit when using V Carve.
I hope this helps to save time and material while minimizing frustration.
Helpful, clear and pragmatic! I have become very fussy about verifying the angle of each critical bit before layout and cut. It has saved me some heartache - and helped me identify suppliers wo can measure angles.
Part of the reason I created the test was that I had a bit which had a very accurate 90 degree angle between the faces of the bit. Unfortunately the carbide was attached to the bit after the 90 was made and the faces were not 45 degrees to the center of the rotation. This procedure will allow a bit to be used even through it may be "off" for several reasons.
Taking this to an extreme - a customer who will remain nameless recently cut his first VCarve Pro job using the wrong cutter and wondered why the results didn't look correct - although it did create an interesting result!
The pictures below show what a toolpath calculated for a 90 degree V-Bit looks like when cut using a 60 degree V-Bit.
Another way to measure the included angle of a V bit.
1. Make a short cut at a known depth.
2. Measure the distance from long edge to long edge, at the surface of the stock.
3. Use your CAD program to calculate the angle from the depth and width of the cut.
Don't forget to account for the flat bottom of most V bits when drawing the cross section of the cut.
this also you can measure to cut a test square and fill it cut this sample, and use a magnifier to see when you measure the bottom
measure the bottom, the top and the dept... as much larger the top and the bottom put in a drawing, and with the measure tool you see the real angle... also this way you can see the tip dia.. the tip only virtually zero... with magnifier you can see it's not...
for engraving, there's a company, bitsbits.net... they have halfround engraver bit... their price, and quality is really good... i just don't say best... i don't want say bad others... ahalfroun of this size about 15 on their site... and in very good quality... this kind of bit works only in wax...
I have a machinist friend and was thinking of getting him to make me of the three sided bits from 1/2" carbide. I am thinking of starting with a 30 degree and if it works then getting some made with different angles. Comments and sugested angles welcomed.
He can provide bits at the stated angle.. I am getting mine in 1/2" but I am sure that he could do them in any size wanted. If I can get him interested in making them anyone be interested and what be a reasonable price? Contact would be directly with him as I have enough to do without taking on another project.
I dont have have an example pic to share today but hopefully tomorrow. I have encountered significant steps when machining aluminum with some of our bits. I checked the angles and they are dead-on 90 degrees. (I run a machine/welding shop). I have worked around it pretty successfully though. On the 1/2" alum I run .100 depth of cuts and you can see the steps. I will usually surface the material .025 deep and do a rough/first v-carve with the tool set at start depth of .000. I will then run a finish v-carve at .025 start depth at full depth pass. I use the nice feature that v-carve and Aspire have that show you the max cut depth and use that value to choose the full pass depth. It works great.
in order to hopefully properly fix the issue I plan to run some sample files and change the angle slightly on each. like 89 or 91 degrees and incrementally after that.
I dont know how significant that is but I thought I would share that.
Perhaps this does have some creative potential. I may set up a variety of bits with incorrect angles to take advantage of the cut. I've been doing something like this by substituting a bradpoint round over while programming for a V bit.