# How do I cut a 16mm 45 degree slope on the sides of a 48mm high square block?

Iâ€™ll leave it to the experts, but it seems to me, if you have a 90 deg V Bit, you could set up a contour on the outer square at a depth of 16MMâ€¦or maybe an advanced V-Carve at 16MM.

3 Likes

I would do a contour cut like Gary mentions, but since a vbitâ€™s tip is not really cutting anything (considering the speed of the cutting edge is almost zero there), a possible refinement consists in using an offset contour and a larger depth (with a little bit of math involved), as in:

There are two ways to do this:

Set up the job:

either do a pair of V carvings along the top and side edges which will cut to the desired depth (draw it up in profile or do the trigonometry to determine this)

Assign V carvings:

Or, if using the new 629:

https://carbide3d.com/carbidecreate/beta

draw a perimeter rectangle:

Then assign a No offset contour toolpath to the desired depth:

As noted above, it would be best to offset these to the outside a bit and overcut, esp. at the corners.

3 Likes

I guess I would need a 90 degree Vee Groove of appr. 1", that is a bit bigger than the Carbide 301 0.5" Vee Groove. Where do I find a 1" 90 deg Vee Groove for Carbide Shapeoko 4 CNC Router XXL (for MDF) ?

I think you only need about 3/4" CH

1 Like

You can use your existing 90 deg bit, but you must get creative in using it! You will need to create additional squares to cut on, but donâ€™t cut as deep. So in the attached example. There are 3 squares drawn each 5 mm apart. The inside square has a cut depth of 5mm, the next out has a cut depth of 10 mm and the outside has a cut depth of 15mm. You end up with a total depth of 15mm all at 45 deg chamfer.

SquareWith45DegChamfer.c2d (15.7 KB)

The simulation in CC 6.29 isnâ€™t quite correct, it shows 2 sides that are not at the correct chamfer, but two that areâ€¦ But you should get the idea. Iâ€™ve used this method a number of times with very good results.

How do you load Amana tools into Carbide Create and Motion ?

Iâ€™m not sure where you get the specifications for the tools you have (Amana site, Iâ€™d imagine), but hereâ€™s a video that describes the process of updating the tool library. Itâ€™s on Carbide Pro - so the version canâ€™t be that oldâ€¦things have changed with the tool menu, but youâ€™ll get the idea:

Shapeoko 4 XXL. I decided to buy a Amana Tool 45718 V Groove 90 Deg x 7/8 D x 3/4 CH that I hope can make it in 1 cut ?

PS. I opened two new treads: How do you make a pocket really precise, hard and smooth in MDF (and don't say sand it)

Is there any reason I can not just draw a rectangle a few millimeter bigger than the original box on all sides and cut after that ?

With the new ability to use V endmills in Carbide Create for Contour Toolpaths that would work â€” showed doing so in the latter portion of the instructions above.

What Amana v groove 90 deg 1/4" shaft should I use if the cutting depth is 3/4" ?

Draw it up in profile:

To do that w/ a single pass you will need over 1.5" of diameter â€” which Amana does not have available in a 1/4" shank tool:

youâ€™ll either need to use multiple tool passes, cut more shallowly, or source a different tool.

Elaire has an 8mm (5/16") collet which may make a larger tool available â€” if you go that route, Iâ€™d still suggest multiple passes w/ the smaller tool â€” just leave a roughing clearance and take the finishing pass w/ the larger tool.

1 Like

Building on what Will did thereâ€¦ (side view) You can do this with your #301 90Â° 1/2" V-Bit

These are just the finish passes, so youâ€™ll want to rough it out to within 2mm first.
This is at 16mm. At 3/4" (19.05mm), youâ€™d want 4 passes

2 Likes

This topic was automatically closed after 30 days. New replies are no longer allowed.