Drawing up a design in profile

[WillAdams (William Adams (Carbide 3D))]

as requested on support…

given the typical sketch:

We need to work out how to cut that as a profile into a piece of suitable material (which is 1.75" thick).

This will require:

Using unsupported tooling in Carbide Create: Roundover / Cove / Radius bits

These are usually used in routers for decorative effects in wood: https://www.whitesiderouterbits.com/products/1570 but they are potentially useful for joinery: They are also useful for rounding off parts to allow rotary motion as for a hinged lid. Unfortunately, Carbide Create does not support this endmill geometry — but using the new support for previewing a V endmill when used in a No Offset Contour toolpath, it should be possible to preview them w/ confidence by stacking a series o…

presumably a 1574 (folks w/ an ER-20 spindle should consider the 1580)

The other consideration is the size of the stock — I am going to assume that this is going to be cut into glued up MDF and that the length will be 4 ft — presumably the CNC is being used to avoid the expense of having a set of molding knives made, or doing multiple setups on a routing table or shaper (cue old joke about a shaper — it’ll make anything but money (due to the expense of tooling and the time and effort of setup/operation)) and only a short length is needed (perhaps it’s part of a door?) which avoids the need for tiling.

Since the piece is symmetrical top/bottom, the assumption is one will do only one side, then rotate it 180 degrees and cut the other, see:

CNC Router Flip Machining

First, we set up the job:

for further details on this see:

https://carbide3d.com/hub/courses/create/job-setup/

Note the setting of the origin at the Top-Left — the assumption is the piece may be taller than the Y dimension specified — this will allow this to vary (the excess height just sticks out the front of the machine) and the origin is at the back left. Similarly, since the job will be flipped, we use half the thickness of the actual stock since we only cut half the design at a time.

Then we draw up the design in profile to get the spacing/depths:

and if need be, reposition it:

The 1574 has a DXF profile available:

which we import:

Deleting what is not needed:

grouping what is left:

and then rotating it and positioning

it relative to the stock:

and nudging it out of the way to the left:

The angle looks to be 45 degrees, so will be cut with a #301 (or other 90 degree tool), so we draw one up:

Done

then draw in a rectangle:

and do Boolean Intersection:

OK

and similarly rotate and drag it into position:

It will be rotated 3/4" from the other tool:

so using the Move command to re-position it:

Done

There will need to be a 3/4" high rectangle for a pocket in-between these twain:

which will need to be wider by at least tool diameter plus 10%:

which should then be centered on the stock:

OK

Similarly, there will need to be a pair of lines which are just a bit wider than the stock (or the rectangle may be duplicated and edited to create two separate lines)

Done

Scale

Done

Again, drag these into alignment with their tool proxies:

and align to stock:

Ok

At this point it is simply a matter of assigning toolpaths, which is pretty obvious, and if desired, adding a set of V toolpaths to approximate the roundover cut.

Note that the #301 is too small to make this cut in on pass, so either a larger tool will need to be used, or multiple passes will be made.

[WillAdams (William Adams (Carbide 3D))]

The toolpaths, as noted, are quite obvious.

It is probably best to cut the profile tools first, but it is probably best to fully draw up the profile — the uncut portion is simple:

A dimension which is not provided is the depth of cut for the roundover tool — positioning it cutting fully down from the surface:

and trying various values:

0.03125" seems about right (1/32")

Done

Drawing a rectangle:

we get the depth, and something which we can use to position the V tool:

As noted, if using a #301, two passes will need to be made:

so we duplicate the tool and position it:

at the center, which then allows us to measure for the depth:

(or one can draw a rectangle for something permanent:

[WillAdams (William Adams (Carbide 3D))]

Duplicate one of the lines to be in-register with this:

and then align it to the stock:

Ok

and then assign a No Offset Contour toolpath:

and repeat that with the other line for a V tool:

with that depth we can also assign a Pocket toolpath to clear the space in-between:

which previews as:

and just leaves the shoulder and the radius tool. As noted, the radius tool cannot be directly previewed, but this may be approximated by a series of V tool previews.

First, the shoulder wants a #251 downcut tool, so we draw it up in profile:

and position it:

and measure for the cut with a rectangle:

and duplicate a line and position it as before:

which previews as:

The actual toolpath for the 1574:

Point Cutting Roundover Bit

is simply another line at that depth:

with a custom tool:

(One option is to use a narrow V tool)

at appropriate feeds and speeds — see the manufacturer’s recommendations and:

Feeds & speeds | Shapeoko CNC A to Z

which previews as:

Adding additional V tools so as to get a reasonable preview is left as an exercise for the reader.

Getting a 3D preview of the G-code is one aspect of a current project which hopefully will be posted presently.