Creation of the CNC Widget.

 

Part 1. The Concept

• Keep it simple think in terms of cutting 1/4” material with a 1/4” straight bit. This will allow a piece of the material to slide into a single straight slot created by one pass of the router bit. If you wish to use slightly thicker material, or a smaller bit, then in order to create a tight fitting connection, you will need to create slots by cutting carefully sized rectangular slots with multiple passes of the router.

• Start with something simple like a small desk shelf/organizer or a table-top napkin holder or condiment container. Then think in terms of what shapes are needed to construct such a thing.

• Once you have a basic object, then expand on your simple concept with other features that improve its function or appeal.

 

 

Part 2. The sketch

• Start with a sketch plan with paper and pencil they are FAST and easily modified, and provide the greatest creative freedom to modify as you go.

• After sketching, show your concept to someone else, you will be amazed at the cool ideas they suggest that you never thought of.

• Re-sketch, move to graph paper and sketch to scale or use 1/4” graph paper, and draw full size if you want. This will really let you see what needs to be done and simplify the CAD process.

 

 

Part 3. The CAD version of your concept

• You need to create a .dxf file and place it on floppy, zip, or cd.

• If you use AutoCAD then when you save your .dxf file be sure to use revision 12 (R12). Also, you may need to Pedit multiple shapes before exporting as version 12.

• Your CAD file must be “clean” without gaps or choppy line segments. Lines, arcs, and shapes must truly connect at intersections. Single shapes or lines are preferable to multiple lines or segments.

• You should be able to use any CAD program that produces .dxf files. However, not all programs have been tested, so be prepared to do some experimenting.

• The next step will be to use “toolpath” software to analyze your drawing. You will probably learn that you need to do some “touch-up” work to your CAD file.

• The manufacturing lab has Inventor 4.2 and Cad Standard Lite installed on the single work station in the Think Tank.

• Visit my website http://tryon.oswego.edu to see the Standard Cad FAQ and links to download the software.

 

 

Part 4. CadStd Lite v3.5.7

• Start with a blank drawing

• In Settings, set the dimensions to Engineering (inches) units

• In Settings, set the paper to the custom size of 21 inches x 21 inches with a scale of 1 = 1

• In settings, set the grid to x=.25 and y=.25

• You are now set to draw.

• Save your work periodically

• Do not use the text tools

• Do not use any spline tools

• You do not need to dimension any drawings for the machine files, although you may want to add dimensions for your own purposes.

• You do not need to use more than one layer for the machine files. Everything can be on the single default layer.

• Line type can be the standard default solid line.

• Line type can be set to auto width

• Layer controls simply allow you to quickly switch between layers and select which ones you want to view.

• Most of the time you will use the snap feature set to “grid”. This will let your drawing objects snap onto the intersections of you 1/4” grid.

• Generally, every tool can be selected from the tool pallet on the right side of the screen. Tools are selected with a single left mouse button click. Then the bottom of the screen begins to show basic instructions. However, most shapes are initiated with another left button click, and ended with another click. The tool use is discontinued with a right mouse button click.

• Basic shapes (as shown by their shape include) arc, circle, oval, line, polyline, rectangle, dimension.

• Basic editing of existing shapes (as shown by their icons include) copy, move, delete, simplify, rotate, mirror, scale, array, change entity.

• Basic window tools include zoom in, zoom out, center window, zoom window, zoom all.

• Clicking one time on the undo menu in the menu bar will undo the last operation.

• Using a right mouse click after completing a drawing operation will quickly repeat using the same tool.

• Drawing (using the line as an example) can be done in three ways. You can click the mouse on a starting point, drag to a new location and then click again to establish the end point. The second method involves clicking on a start location and then entering a value in the “X” box (x axis offset distance) striking the TAB key to move to the “Y” box and entering a value (y axis offset distance) striking the ENTER key to draw the line. You can then continue to enter x & y values to draw lines around using only the value entry boxes. The other value entry boxes are DISTance & ANGle. These are greyed out because you can use either the X & Y boxes OR the Dist & Ang boxes. The unused set will be greyed out. You can enter a distance in the Dist box, press TAB and then enter an angle in the Ang box, and strike the ENTER key. Your line will be drawn the distance and at the angle you specified from the previous starting point.

• Practice some simple drawings first. It takes only a few hours to become very proficient with this CAD package.

 

Part 5. Your finished CAD files

• Save your CAD file to your floppy or zip disk. This will save it as a .cad file.

• EXPORT your CAD file to your floppy or zip disk. This will let you select .dxf as the file format.

• Be careful with your magnetic media disk.

• The next step requires that you use “Toolpath” to open your .dxf file and create the machine (.rdy) file. However, save your .dxf files since you will need to upload them to the webserver along with the completed .rdy files.

 

Part 6. Toolpath

• Open toolpath and select the .dxf file that you would like to work on. Unless you are using the machine connected to the router, Toolpath may give you an error message saying that “No Machines Are Available”. This is fine, you can still use Toolpath to create and save the needed ready file (.rdy)

• If Toolpath is open then use the FILE menu and IMPORT a .dxf file to work with.

• When your file comes into Toolpath it will be sized to the extents of your drawing. Paper size means nothing in Toolpath. It will place a dotted yellow border around to outer-most area of your file. This will be the physical size of your file. If you notice that shapes are poorly arranged, then you may wish to go back to your cad program to turn, rotate, or move any shapes that need adjustment.

• Shapes come into toolpath as one of three types: Open shapes are green and are only objects like straight or single lines. The router will travel right down the center of open shapes. Outside shapes are blue and represent actual parts. The router will want to travel on the outside of the blue line, thus creating a shape exactly the size that it was drawn. Inside shapes are shown in red. These are shapes that Toolpath interprets as holes. The router will want to travel on the inside of the red line, thus creating a hole exactly the size that it was drawn. DO NOT be concerned if shapes are the wrong color when you first import a drawing into Toolpath.

• The first action you need to perform is ANALYSIS. Click on ANALYSIS and a window will open that shows various cutting errors. You will click on all four of the top buttons (Open Shapes, Duplicate Shapes, Direction Errors, Sequence Errors). This will force Toolpath to take a second look at all the shapes and re-evaluate which ones should be open, inside, or outside shapes. This should clear up all problems with shape classification.

• Now all of the holes should be in red, the parts in blue, and the slots in green. A common problem at this stage is discovering a hole or a part is shown in green. This indicates A PROBLEM WITH YOUR CAD FILE. You will need to go back to cad and fix that shape. Most common errors that cause this include:

            - Duplicate lines on top of each other.

            - Lines that don’t actually intersect at their endpoints.

            - Lines that were not grouped with the Autocad P-edit command.

            - Autocad drawings that were not saved as version R12 .dxf.

            - Shapes created in Autocad that were created using the boundary tool.

            - Shapes created using a spline tool.

            - Shapes created or modified with the chamfer or fillet tool.

• After the analysis is complete parts should be place into groups if necessary. Groups are only necessary if shapes in your project need to be cut to different finished depths. For example, if you are producing an engraved white board then the engraving shapes are called “pockets” since they will not be cut all the way through the stock. The overall whiteboard shape and any mounting holes in it will be cut through the stock. Therefore the two collection of shapes will need to be in different groups.

• IF necessary, click on groups and select MOVE TO GROUP or COPY TO GROUP. Then carefully click on every shape that you wish to move. Click on TO GROUP and select a color group to move or copy the shapes to.

• Groups are made visible or invisible by going to the OUTPUT menu and switching the “Machining Path” from forward to off.

• All shapes must be SEQUENCED. Go into the EDIT menu and select SEQUENCE. Then click on each shape in the order that you want them cut. Obviously you should work from the center of each shape outward. Do not cut a part loose of the stock and then try to cut a slot in the loose part.

• You should also try to work from the far side/end of the stock back toward the clamps that will hold the stock.

• After clicking on every shape, you must click on the FORWARD button. Then it is a good idea to repeatedly click the NEXT button and watch carefully as Toolpath highlights, in order, the shapes that will be cut.

• The next step, in the edit menu, is to change the START points if necessary. Click on START. This will show where the router will start every shape. The yellow flag shows the start location and points in the direction of travel. Start points should be placed away from complex areas of each part and in a location that simplifies the needed finishing operation. Simply click on the area of a shape where you want to start point.

• Next return to the edit menu and then to the main menu. IF YOU HAVE MORE THAN ONE GROUP YOU NEED TO SEQUENCE EACH GROUP AND THEN SEQUENCE THE GROUPS THEMSELVES. In the sequence menu you can click on “BY GROUP” and select the cutting sequence of each group.

• From the main menu, click on OUTPUT. You will need to set the bit compensation. The router needs to know the radius of the bit you will use. In other words, how far from the center of the drawn lines will the bit extend. Locate the radius of the bit (if you will be using a 1/4” bit then click on the plus sign next to .125) and click on the plus sign.

• The machining path should be set to Forward.

• Depth should be set to THRU unless you are setting a group for a pocket. Click on the word THRU and enter a decimal inch depth (for 1/8” enter the decimal .125).

• Multipass is only used when cutting thick stock (greater than 1/4”).

• That is it, now change the JOB NAME to an 8 character name that is easy to recognize and click on the “Save Ready File” button. Navigate to the disk or folder where you want the file. This will create a .rdy file.

• After the save, you will be returned to the output window. Now click on the “Send” button and you will see the machine file that the router will see. Check that all the shapes are shown. If the file looks fine and you are working on the machine connected to the router, then click on TRANSMIT. A status bar will scroll across the bottom right of the screen as the job is sent to the router.

 

 

Part 6b. Toolpath Summary

1. Import File

2. Analysis

3. Group (if necessary)

4. Sequence Shapes

5. Start Points

6. Output (save .rdy file)

7. Output (send .rdy file)