5º bevel on part

[daveanddanyelle]

Hi Everyone,
I'm still fairly new to CNC'ing and VCarve 10.5, so I'm hoping the folks here on the forum can save me some trial and error time as well as wasted material (not to mention frustration).

I need to make a part which is a template for a bearing to follow on a machine I'm making. The part is an oval 2"x4" and will be .75 thick. Basically a rectangle with a semicircle at each end. The part needs to have the sides tapered at 5º. I have a 5º bit. The part needs to be 2"x4" in the middle of the taper. That way, if the piece being created from the template part needs to be bigger, I just move the follower bearing down toward the fatter part of the template part, and if it needs to be slightly smaller, I can move the follower bearing up a skosh. I'm attaching (hopefully) a rough drawing.

and with a sad attempt at depicting bearings...

I can draw the shape I want well enough as a 2x4 oval, but I think that if I do that, and then use the 5º cutter, I will end up with the bottom of the template part being 2x4, and the middle being somewhat less than that. I suppose I can use 3d modeling software to create what I'm looking for, then measure the bottom of the 3d model and get a new size for the part, but was thinking it might be a good learning experience to try it from within VCarve.

My question is... is there a practical way to make the software do what I'm describing without doing the math or additional drawing?

Thanks for any suggestions!

[adze_cnc]

Create a Profile toolpath using the tapered cutter and using 'Outside' for "Machine Vectors..." setting?

[jerry carney]

I agree, that should work.

[litzluth]

Dimension wise, I think this is the solution, but someone who wasn't mostly staring out the window in 9th grade trigonometry class (unlike me) may want to check this.

You know the angle (5 degrees) and the adjacent (3/8"--you might think 3/4", but you want the run from the middle of the part, not the top) and you want to calculate the opposite. I get 2" + (.032808248822222 *2) for width and 4" + (.032808248822222 *2) for length at the bottom of the part, cutting outside the vector, like adze said.

https://keisan.casio.com/exec/system/1223010584

[daveanddanyelle]

Thanks Guys.

Adze, thanks for your reply. I think it brings up a question for me, that I'll ask below.

So Litz, I get the same numbers when I did both the math as well as a 3d drawing. For my purposes, .033. So what I think you are saying is to add .033 to each side/end, so have an oval of 2.066x4.066 and then cut outside the line with the 5º cutter?

So new question then, and I suppose this is in the literature somewhere... if using a 5º bit, the bottom of the bit is something like 3/8" and the top is 19/32" (based on the box dimensions). I haven't added any "unique" bits to the tool data base yet. Just basic straight end mills or ball nose EMs. Would I then just add this as an end mill, noting it is 5º in the title, and enter the diameter as 3/8" (.375)? or is there a particular way to do things such as tapered bits? I see bits can be entered as profile bits...?

Would it be advisable to do a rough cut and then do the bevel with this bit, or just do multiple passes with the 5º? I ask because my 1/2" straight bit cost like $12, and the 5º bit is $50. So if going to wear a bit out, I'd rather it be the $12 one.

Thanks again for the help,
Dave

[adze_cnc]

It’s not really about trigonometry. It’s about the Profile toolpath cutting on the Outside of lines. With a properly described tool the Profile toolpath cutting to the Outside of a line will never cut too small or too large at the top of the material (presuming the “Allowance offset” in the “Machine Vector…” area is set to zero.

VCarve takes care of the math.

Would I then just add this as an end mill, noting it is 5º in the title, and enter the diameter as 3/8" (.375)? or is there a particular way to do things such as tapered bits?

There are three (actually four) bit types that can be tapered:

1. V-Bit: when the two sides meet at the tip (think the vertex of a triangle)
2. Tapered Ball Nose: when the two sides meet at a rounded tip. https://www.amanatool.com/pub/media/cat ... /46256.jpg
3. Engraving: when the two sides meet at a flat tip

Create your 5 degree as the one closely matching one of the three above.

What’s the 4th type? The “Form Tool”. This is for when you have a profile that doesn’t match the three above. For example a bit that tapers at 5 degrees and then near the tip tapers again at 45 degrees to a point (if one such bit exists).

Would it be advisable to do a rough cut and then do the bevel with this bit, or just do multiple passes with the 5º?

I don’t know your bit or your machine’s capabilities. Personally if I were to pre-rough out for the tapered bit I’d use a V-Bit (60 or 90 degree included angle) and use a Profile toolpath “Outside” the line to let VCarve figure out the cut.

If you do use a straight bit then you’ll have do the trigonometry to figure out how much to offset your vectors to make sure you don’t impinge on the bottom of the tapered cut.

Remember, though, if you are using a tapered ball end you have to account for that rounded tip too.

Steven