4 Axis Saw

RcimCycles_094

This cycle is set up much the same way as a normal straight cut, except use the tool number for the four-axis saw head. Router-CIM will interpret the axis geometry and all moves required to complete the cycle. The Control Panel settings for this cycle are the same as for a 2D cycle.

• The 4 Axis Safe field has no function in this cycle.

• The Saw Offset field is used to determine the distance from the center of the saw to the center of the blade.

• Cutter Compensation is available in this cycle.

Download sample drawing here.

The saw offset 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.

For a saw, you might want the tool path set on top of your geometry with no offset (use 0) or offset by some amount relative to your saw spindle or aggregate.

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

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 (in inch mode). 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.

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.

Setting a number between 0 and 1.0 will give you a percentage of the max feedrate (for instance 0.4 would be 40%).

Setting the number to a value greater than 1.0 will give you an exact feedrate. For instance 250. would generate F250. in the code.

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.

**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.