The AvCAM operating system for the Panel Pro will automatically provide tool paths on the correct side of the line for inside and outside cuts in the auto tool path mode.
For auto tool path to work, it must be able to join a series of lines and arcs with end points that do not have gaps or overlaps of more than .005″. five thousands of an inch represents pretty sloppy drawing and we can do better using the precision drawing aids provided by most modern CAD programs.
When AvCAM joins the end points, it uses the first entity on a selected drawing layer. It then uses that line or arc end point to match a starting coordinate of another entity. If there is not a starting coordinate that matches, it will look for an ending coordinate and so on until it makes a closed poly-line. This poly-line may be either clockwise or counter clockwise and it is AvCAMs responsibility to determine which way it is going with reference to its center.
Because of tool deflection we need to cut inside cuts counter clockwise and outside cuts clockwise. We inform AvCAM that we want a cut to be clockwise by putting its entities on a layer called “outside”. If a poly-line is determined to be going the wrong direction, AvCAM will reverse it. The problem still remains of determining if a figure is rotating cw or ccw about its mid point. Most Instrument cutouts and instrument panels have fairly regular outlines that can be readily determined. Without going into a dissertation on poly-line direction algorithms, there are some figures that the direction cannot be determined and manual tool paths will need to be supplied.
This is an example of a figure that cannot be resolved. Even though its layer is outside, AvCAM simulates and cuts on the inside. It is intended that is to be cut out and used to fill an unused knob notch. The size is approximately .4″ high by .3″ wide. To cut this figure, we will need to resort to the AvCAM classic mode.
The following are instructions on how to use the classic mode.
Another example of where you would want to use classic mode is where you want to produce a tool path on a line or group of lines that do not form a closed figure.
The classic mode has tool paths created by the drafts-person on their own layer. The naming of the layer is irrelevant.
The first thing you need to do is check that the line segments are pointing in the correct direction. In AutoCAD or DraftSight use the entities properties to show what the bearing of the line is. In EasyCAD use list > info and towards the bottom of the information is the bearing. Generally just knowing what quadrant the bearing is in is sufficient to determine if the direction is suitable.
If a line is not going the right direction, it needs to be changed. Frequently the easiest way to do this is to erase the line and draw a new one using existing geometry to snap to.
Arcs always save to the dxf rotating counter clockwise. We will deal with them when we actually make the tool paths. It is just easier to have the lines going the correct direction to start with.
Before we proceed, we need to do something about the 2 little arcs at the top and bottom left of the drawing. We cannot physically cut an arc whose radius is smaller than the radius of the end mill used. In this case, the arcs have a radius of .019″. Even a 1/16″ end mill has a radius larger than that. What I would do is to remove the arc and replace it with a straight line which will be a bit easier to deal with. I erase the arcs and replace them (going the correct direction) snapping to the end points of the existing entities.
It is now time to create our tool paths. Create your tool path layer. I called mine 0938 because I am going to use a 3/32 (.0938) inch end mill.
EasyCAD has a offset chain command that will offset and trim a series of connected points. Because some of the entities to offset are very small compared to the offset value, even EasyCAD cannot resolve the issue. We need to offset each entity and trim as appropriate. When EasyCAD offsets, it creates new entities that use the currently selected layer, color etc, so it is good to have these set up before offsetting. AutoCAD and most others make new entities that copy all of the properties of the entity being offset. The layer will need to be changed after the offset. In either case the geometry other than the offset location is copied.
This is what our offsets look like. Use the EasyCAD trim to intersection or AutoCAD fillet (setting radius to zero) to trim these to their intersections. Take care where the lines meet the arc on the right because there is an overlap. The almost straight line on the left side is an arc that will rotate ccw with respect to its center. The arc on the right will need to rotate cw with respect to its center. Since all arcs save to dxf rotating ccw, we use the cyan color to inform AvCAM that we want this arc cut cw with respect to its center.
Cyan is a specific color just above yellow on the EasyCAD color bar, not just a light blue.
This is what the drawing looks like after trimming and changing the cw arc to cyan.
We have just one more step to complete. Setting the order. Classic mode cuts the entities on the selected layer in the order and direction they occur in the dxf file. EasyCAD has a command called front. Assuming you have the extended commands set up on EasyCAD, it is the icon “F” on the left side, or edit > front on your menu.
To front the toolpath: open the front command. left click on the first entity to cut. observe that that entity has changed to your selection color. right click or hit enter to complete the command. the selected entity returns to its original color. Right click again to re-enter the front command. left click on the 2nd entity to cut. right click
Repeat until you are all the way around the figure. zoom in enough that you just select one entity at a time. When you are done, save it as a dxf.
To set the order in AutoCAD. click save as. select files of type DXF. in most cases an AutoCAD version of R12 is preferred for cutout work. It seems like each version of AutoCAD has a different look to its SAVEAS dialog, but somewhere there will be a “tools” button or drop down. click it. click dxf options. the ascii format should be checked as well as select objects. click ok to exit the dxf options, then click save on the SAVEAS dialog. You will then be asked to select the objects. Click on each entity in the order you want them to cut. When you are done, all of the entities you want cut will be highlighted. hit enter.
AutoCAD holds a dxf file open while it is displayed on the screen, so you will need to close the file in AutoCAD before opening it in AvCAM.
open the file.
select only the tool path layer.
open the cut dialog. select the classic mode. Note that in classic mode the end mill size is used for display only and does not affect the cut.
Simulate. Note that the simulation proceeds along the center of the line. If it skips a spot or goes backwards, you need to go back to CAD and fix it there.
Now, aren’t you glad you have AutoToolPath for most work?