|
|
|
|
|||
|
|
|
|
|
These cut cycles will allow the tool to start at the center of a circle, plunge down to the cut depth, interpolate the circle back to the starting point and then move back to the center of the circle and retract to the safety plane. The difference between them is that Hole Interpolation 2 will have an overlap in the cut past the start point before the tool moves back to the center of the circle.This cycle only works on circles or arcs.You should only use this cycle when there will be no slug left behind in the hole that could be expelled from the part and cause injury. |
Hole-Interpolation 1 tool paths.
Hole-Interpolation-1 Parameters
The following parameters effect the toolpath creation:
Offset Dim
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 the Offset Dim section for more information.
Cut Direction
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.
Lead Feed
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.
See the Lead Feed 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 x4.0 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. Entering a negative number will move the tool path DOWN in Z.
See Z Stock Allowance 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.
