2D Profile Cutting

2D Profile Cutting is used to cut shapes out of material. 

2D Profile Cutting requires closed, planer polylines or curves. The tool will follow a path half of its diameter (plus Stock to Leave if specified) offset from the selected curves. 

You will need to place the curves to be cut into the following layers in the Rhino document:

KaroroCAM/2D Cutting/Inside Curves - for curves to be cut to the inside of the curve

KaroroCAM/2D Cutting/Outside Curves - for curves to be cut to the outside of the curve

USE CLIMB CUTTING

Checking this box will change from Conventional to Climb cutting.

NOTES: Climb and Conventional cutting merely describe the way in which the cutter moves around the part in respect to its direction of rotation.

In regards to a right-hand rotation spindle (the most common type), moving around a finished part counter-clockwise would be considered Conventional Cutting while a clockwise part path would be Climb Cutting. The terminology will be reversed if the spindle is of left-hand rotation or a pocket or hole is being cut out of the finished part.

The main difference between climb and conventional cutting is how the cutter bites into the material.

A conventional cut deflects the bit towards the cut and a climb cut pushes the bit away. Climb cutting can be dangerous on a non-CNC router, as the piece may he hard to control by hand and may ‘walkaway’.

On CNC routers, the harder materials such as Aluminium, Solid Wood and Hard Plastics (Acrylic, Polycarbonate, Nylon)) generally leave the best finish with a climb cut set up. However on softer materials and Laminates like Soft plastics (HDPE, UHMW, Polypropylene, etc.), Plywood and Laminated boards, a conventional cut is recommended.

Typically Climb Cutting will only show an improved performance in the smaller diameters (less than 10mm), but of course there are always exceptions.

A quick rule of thumb is to check your offcut. If your offcut has a nicer finish than the part, rotate around the other way and the better finish will be on your part.

Tolerance

KaroroCAM uses polylines (collections of line segments) to create toolpaths. All curves are converted to segments using this Tolerance setting as a guide. The Number represents the maximum deviation from the input curve to the final polyline.

The green toolpath curves in these two pictures show the extreme of the 1mm vs 0.001mm settings:

TIP: Use a tolerance one decimal place better than your machines smallest movement step - ie for most CNC routers 0.01 is recommended Tolerance

NOTE: Tight tolerances can lead to large file sizes and slow machine movement while cutting 

Outside Corners

This menu allows you to switch between Sharp and Round outside corners on your toolpaths. 2D Profile Cutting toolpaths are an offset from your input curve - based on the tool radius and stock to leave settings - with the two options being the difference in how offsets can be calculated on external offsets. 

NOTE: Rounded corners tend to be a better choice on angles less than 90 deg. Sharp corners can lead to smaller G-code files on cutting jobs that are mostly 90 deg corners.

NOTE: Rounded corners are effected by the toolpath Tolerance setting. 

Tool

Tool Shape

2D profile Cutting is done with a Flat End Mill:

Tool Diameter

Sets the diameter of your tool bit in mm.

Tool Number

Select Tool number that matches the tool spec'd in your tool path - mostly important for machines with auto tool change ability.

Spindle Speed

Sets the spindle speed for this operation in your GCode output file

Stock to Leave

Stock to Leave

This setting allows you set an additional offset to you cutting path to leave some extra material on your job.

TIP: This setting can be used to produce a better surface finish on your job, especially on jobs that require Multiple Depth cuts. Leave say 1mm of material on initial cut which can be removed on a second, net sized cut at full depth. The smaller amount of material removed on this second cut usually leads to a cleaner finish

Cutting Depth

Cutting Depth Position

Selects the reference position for the cutting depth. Can be:

Selected Curves - the cutting depth will be referenced to the curves in the Inside Curves/Outside Curves layers in the Rhino document. These can all be at different Z heights

Stock Top - Cutting depth is referenced to the top of the current stock - all cutting will be done to the same depth

Stock Bottom - Cutting depth is referenced to the bottom of the current stock - all cutting will be done to the same depth

NOTE: Cutting Depth Offset is a Z offset from this selection

Cutting Depth Offset

Offset in mm in the Z direction from the selected Cutting Depth Position of the final cutting depth. 

Multiple Depths

USE MULTIPLE DEPTHS

Check this box to enable multiple depth cutting

Max Step Down

Maximum step down in mm per pass when doing multiple depth cutting. 

NOTE: If the total cutting depth (Stock top - Cutting Depth Position + Cutting Depth Offset) is not an even division by this number the deepest pass will be less than this number.

ORDER CUT BY Z DEPTH

Check this box to order cutting by Z depth rather than per outline when doing multiple depth cutting. 

NOTE: This can be useful on machines with vacuum hold down to not 'break' the vacuum on the parts until the final depth pass

Ramping

USE RAMPING

Check this box to enable ramping tool entry into the stock.

Ramping Angle

Sets the angle the tool will enter the material at the start of each cutting pass.

NOTE: You may get a warning if one or more of the cutting paths is too short to contain the ramping motion. Either increase the ramp angle and/or reduce the cutting depth per pass to allow for a ramping motion that is suitable for your 2D profile. 

Post Process

Post Process 2D Profile Cutting

Click this button to proceed to the Post Process Selection and Gcode File saving

VIDEO - 2D Profile Cutting in KaroroCAM