Ramp Outside Partial cutting cycle allow you to have a helical lead-in and lead-out from a point perpendicular to the part. This cycle is especially useful to save on tool wear, and in circumstances where the cutter cannot plunge into the material. This cycle will also let the user define an offset so that the ramp lead-in and lead-out will be at the Total Cut Depth prior to moving into the part edge helping prevent deformations on the bottom of the parts.
Ramp Outside Partial will only work on closed shapes, and produce cuts with an offset to the outside of the geometry according to the cycle.
The tool will start above the part at the Safety Plane, and then make a linear ramp lead-in to the Total Cut Depth defined and will be offset from the edge of the part by the LeadOffset parameter. Once at depth, the cutter will follow a 90° arc to complete the lead-in ending up at the edge of the part and cut back to the start point, overlap the start point, make a 90° arc away from the part edge and then make a linear ramp lead-out back up to the Safety Plane.
Ramp-Outside Partial cycle
Ramp-Outside Partial (from above)
There are several parameters set by the cycle as defaults, and most will not need to be changed. The valid parameters are shown below:
Note: In order to use this cycle, LeadOffset and Ramp Amt. need to be properly defined.
Ramp-Outside Partial Cycle Parameters
The following parameters effect the toolpath creation:
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.
See Offset Dim for more information.
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).
See the Cut Side section for more information.
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.
See the Cut Direction section for more information.
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.
See the Round Corners section for more information.
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.
See the Lead-In section for more information.
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.
See the Lead-Out section for more information.
Use Lead Size to change the length of the leads. The default for this cycle is 1.0. 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.
Note: Changes in the Lead Size will scale the LeadOffset proportionally.
See the Lead-Size section for more information.
The Lead Angle for this cycle must be set to 0.0.
See the Lead Angle section for more information.
XY Stock Allowance
Placing a value in this parameter will offset the tool path to leave material for a finish pass. For instance, placing .125 in the XY Stock Allowance and cutting a 6.4 x 4.0 shape will actually leave a part that is 6.25 x 4.25, by adding .125 to the offset of the tool path all the way around the part.
See XY Stock Allowance for more information.
Z Stock Allowance
Placing a value in Z Stock Allowance will change the Total Cut Depth by the number entered. You can use this if you want to leave a small amount of material on the bottom of a part, or if you intentionally want to overcut a part to be sure it is cut all the way through.
Entering a positive number will move the tool path UP in Z, leaving more material for a finish pass.
Entering a negative number will move the tool path DOWN in Z, past the normal Total Cut Depth.
See Z Stock Allowance for more information.
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.
See the Lead Feed section for more information.
This sets the amount of offset used when the cycle has completed the linear ramp lead-in and starts the 90° arc into the part edge. This field must be a positive number. The larger the number used, the larger the 90° arc will be.
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.
See the Safety Plane section for more information.
Depth Per Pass
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.
Total Cut Depth
The Total Cut Depth is the depth you wish to Cut to based on the top of the geometry, regardless of the number of passes made. Router-CIM uses this number to calculate the Z axis moves for the Total Depth to Cut into the material. If the Depth Per Pass field has a number smaller than this, Router-CIM calculates the number of passes necessary to reach this depth.
See the Total Cut Depth section for more information and the options available.
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.
Ramp Amt determines the angle of the ramp in Z during the lead in and lead out. The default value should be 2.0. You can specify the Ramp Amt as a number that reflects the percentage of the angle from its default. That means that if you want a lead that is twice the normal ramp length (shallower angle) enter 2. If you want a lead that is steeper than the default, enter .5.
See the Lead Ratio section for more information.
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.
See the Overlap Amt section for more information.
**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.