Multi-Pass-Outside

RcimCycles_075

This cycle allows for a rough cut and finish cut on the outside of a shape according to dimensions that you specify in cycle parameters. The cycles creates multiple, offset toolpaths from the outside of the shape towards the finished edge, with specified dimensions for the amount of the first pass, last pass, and cut spacing. You also specify how far away from the finished edge the finish pass is created. The tool will start at the Safety Plane, Plunge to the depth specified in Total Cut Depth or Depth per Pass and then make a straight lead in to the location of the first pass set by the Max Offset. The cutter will make the first pass, then step in towards the finished edge according to the XY Step amount and make another pass until it reaches the offset for the Last Offset. On the Last Offset, the tool will move back and over to a point where it can make a 90° lead-in arc, then cut the finish pass back to the start point, overlap the start point by the tool diameter and make a 90° lead-out arc before retracting back up to the Safety Plane.

Download drawing here.

This cycle will only offset shapes that can be offset in AutoCAD, and if the AutoCAD offset command fails, so will this cutting cycle. There is no provision for leaving 'islands' or separate areas that are uncut in the shape. This is not a pocketing cycle. There are some cut properties unique to this cycle, each of them is explained below.

The offset dim is the amount the toolpath is offset from the original geometry or Geoshape.

Normally this is set by Router-CIM depending on a number of features such as the Cutter Compensation setting and the cut cycle itself. For instance if Cutter Comp is set to Yes, then the toolpath will lie directly on top of the Geoshaped geometry with no offset.

You may substitute the parameters here for numeric values to suit you particular cutting needs.

The value set by default (firstxy xycutloc) is a macro setting that allows Router-CIM to handle the offset automatically and will usually not need to be changed.

Cut Side is the side of the Geoshape that the toolpath will be created on. For instance Plunge-Outside (Plunge-O) will have the toolpath on the outside of the shape. Valid entries for this field are Outside, Inside, RH (Right Hand) and LH (Left Hand).

The direction of the cut can only be clockwise (CW) or counter-clockwise (CCW). This even applies to open shapes where this direction really has no meaningful relationship to the geometry selected. Any closed shapes should have the direction set accordingly and any open shapes should be set to CCW as all shapes in AutoCAD and Router-CIM are CCW by default.

If set to Yes, this option will round sharp corners with a radius of the value stored in the task *cutfil*. The default is 0.01 radius. This option will insert a fillet in all corners, so if you have an inside cut you will most likely cause an error when the tool tries to fit into that radius. If you have inside and outside cuts on the same shape and need to fillet the corners, use the AutoCAD Fillet command, then Geoshape and Cut the shape.

This field defines the lead-In block name. There are several available, but only some cycles will respond to the change of the Lead-In edits. By default this cycle will usually not have the lead-in or lead-out changed as the defaults will accommodate multiple depths per pass and cutting on any plane.

This field defines the lead-Out block name. There are several available, but only some cycles will respond to the change of the Lead-Out edits. By default this cycle will usually not have the lead-in or lead-out changed as the defaults will accommodate multiple depths per pass and cutting on any plane.

Use Lead Size to change the length of the leads. This field will affect both lead-in and lead-out if you put just one number in this field. You can put two numbers in this field, separated by a space, and the first number will affect the lead-in and the second will affect the lead out.

Use Lead Angle to change the angle of the lead-in and lead-out. This field also will affect both lead-in and lead-out angles if you put just one number in the field. You can put two numbers in this field, separated by a space. The first number will affect the lead-in angle and the second will affect the lead-out angle.

Max Offset is the distance from the start point to the start of the first pass on the cut. If the cut cycle is Multi-Pass Inside, then the Max Offset will be to the inside of the shape by the specified amount. If the cycle is Multi-Pass Outside, then the Max Offset will be from the start point to the outside of the shape by the Max Offset amount. This is only the distance for the first cut. All subsequent cuts will be determined by either XY Step or Last Offset.

The XY Step is the distance between each tool path from the first to the last (excluding the finish pass) on the Multi-Pass Inside and Multi-Pass Outside cycles.

You can specify the distance as a numeric value, or you can make a task to calculate a step over amount and place the task name in the XY Step field. An example of a task is TW80, which looks at the tool diameter field and then places an amount equal to 80% of that value in this location.

The Last Offset is the distance from the finish pass to the edge of the shape being cut. This can be any numeric value, but if it exceeds the XY Step value, the cutter will not contact the part on the finish pass. Typically this is set to the radius of the tool in a rough-cut, finish-cut scenario. You can leave some material on the part if you want to clean up the part with a finish cutter.

This sets lead-in and lead-out feed rates. The default is 0.5, Router-CIM's standard 50% feedrate for lead-in and lead-out. Whatever number you set this variable to is a percentage of max feedrate set in the Control Panel. Setting the number to a value greater than 1.0 will give you an exact feedrate.

The safety plane is the location in the Z axis where the tool can retract to between cuts.

This should always be a value that places the cutter above the part to be cut as each tool change, or index move between cuts is going to start from this point.

Placing an asterisk ( * ) before the number specifies that this value is an absolute point above the part, where leaving this out determines the point to be incremental.

This field allows multiple depths of Cut in a single tool path. By setting this number to a value less than the Total Depth of the Cut, you will have multiple passes in the material.

For example, if you have 1" thick material and need to take three passes to Cut through, you would set the Depth/Pass field at .4 (any number between .35 and .5 is valid) and the Total Depth at -1.0. The code generated will produce the first pass at -.4, the second at -.8 and the third pass at -1.0.

In most of the standard Router-CIM cycles the tool paths will ramp down between the Cuts.

The Total Cut Depth is the depth you wish to Cut to, regardless of the number of passes made. It is usually put in as a negative number because Z0 is set at the top of the part. Router-CIM uses this number to calculate the Z axis moves for the Total Depth to Cut into the material. If the Depth/Pass field has a number smaller than this, Router-CIM calculates the number of passes necessary to reach this depth.

You may enable Router-CIM to calculate the depth automatically for you based on the thickness you give a part. To do this place "A" in the Total Cut Depth field, and if you have given you part thickness, Router-CIM will use that value for the Z depth. Remember to give your part negative thickness!

Also, when you give your parts negative thickness, you can use a forward slash (/) followed by a negative value (-.01 for example) in this field. Router-CIM will take the negative part thickness (-.75 for example), and the negative value following the slash and calculate the Total Cut Depth. In this case the part would be cut to -.76.

This field specifies the cutting maximum Feedrate in either inches per minute or millimeters per minute, depending on the mode you are programming in. See the chapter on Advanced Settings for information on how to program variable feed rates.

This field sets the spindle speed in rpm's (revolutions per minute). This is a modal field to many machine tools, so if you do not change this field for each Cut with the same spindle, you may only see the output for this setting once although you have made more than one Cut with the same spindle.

Values placed here will be output in the cut cycle before the tool enters the material, typically at the height of the Safety Plane once the tool length compensation is set.

Values placed here will be output in the cut cycle after the tool has retracted from the cut, typically at the height of the Safety Plane after the cut is finished.

A numeric value to use for the tool path created to allow the Sequencer to place cuts in a specific order when the code is created.

Overlap is the movement of the cutter past the starting point of the cut. By default the Overlap amount is equal to the diameter of the tool. You are able to specify a larger or smaller amount for this by placing a value in this field. For instance, if you are using a 0.5" router bit, the Overlap distance is 0.5". If you put 1.0" in the Overlap Amt. field then the Overlap will be 1.0". This is typically done to reduce any witness mark in the material left by the tool on the lead-in maneuver.

**Changing values in the cycle parameters may yield unexpected results with some settings or on some geometry. Examine the toolpath and NC Code carefully before running your machine tool if you change these default settings.