From Qwiki

This is the HOWTO for circuit creation using the LPKF Circuit Plotter.

Contents 1 Altium DXP: Circuit CAD 1.1 Schematic Capture 1.1.1 MabuchiLab Library 1.2 PCB Layout 1.2.1 Rules 1.3 Tips 1.4 Exporting 1.4.1 NC Drill Files 1.4.2 Gerber Files 1.4.3 A SPECIAL NOTE: 2 CircuitCAM 2.1 Importing 2.1.1 Gerber Files 2.1.2 NC Drill Files 2.2 Rubout Areas 2.3 Isolation 2.3.1 Main Tab 2.3.2 Advanced Tab 2.4 Routing 2.5 Exporting for Board Master 2.6 Tips 3 Board Master 3.1 Importing the CAM File and initial setup 3.2 Tool Setup 3.3 Milling 4 Additional Information 4.1 Tools 4.2 Preparing Board

Altium DXP: Circuit CAD

The design cycle typically begins with Altium DXP. This software package can be used for schematic capture, PCB layout and SPICE simulation. Only the first two are relevant to the current article and so SPICE modeling will be left to an other Howto. If you are familiar with DXP, I would suggest jumping ahead to the section on Exporting for CircuitCam.

Schematic Capture

DXP is both a wonderful and terrible piece of software. It's wonderful in that it is powerful and can really help to streamline the entire design cycle. It is terrible in that it can be a bear to use and isn't always intuitive, or always isn't intuitive, or something like that. A few tips:

• To get rid of the annoying fast pan, go to tools/preferences and set ‘auto-pan step sizes’ = 1.
• To make the grid finer/coarser (this determines the resolution with which you may place components) go to ‘design/options’, pick the ‘options’ tab, and then change the ‘snap’ size.
• Make sure to give each and every component a unique identifier (U2,R3 etc) or else the conversion to a PCB will do strange things.

MabuchiLab Library

We are in the process of putting together a single library with the components that we use (with the right footprint etc). For information about contributing to the library go to Managing DXP Libraries. The Library is FatherLoad->Projects->Electronics->MabuchiLabLibrary.LIBPKG and will hopefully contain what you need.

• The POT footprint matches the footprint of our POT's with in-line leads: matching the standard Bourns type 3296 footprint.
• Surface mount component footprints are "0805" for standard caps, "1206" for standard resistors, and "SO-8" for standard Op-Amps.

Here are some hints:

• The bundled PCB libraries are located in "Program Files->Altium->Libraries and non-specific libraries are in the PCB subdirectory.
• Not everything is in the libraries. Many vendors supply footprints (use PROTEL footprints) and schematic symbols which will make things easier. However, it isn't difficult to create a component de novo. The built in DXP tutorial will walk you through the process. All new components should go into the MabuchiLab Library.

PCB Layout

Before taking any steps to create the PCB, decide if you will want to have the option of sending the board out to be manufactured. If you are, read the article preparing a circuit for outside fab.

When putting together a complete design (schematic to board) it's a good idea to keep things together in a project, this will allow you to automatically update your PCB from the schematic and vice versa (to a certain extent) Once you've created your Schematic, create a PCB and save it (Project/Add To Project), then select the schematic and "Design/Update PCB -name- from Schematic" to have DXP automatically drop your components on the PCB. (DXP Bug Note: if you have more than one schematic, DXP will use the schematic at the top of the schematics list in the project window, no matter what schematic you happen to be looking at at the moment. You can reposition the schematics in the list by clicking and dragging. Don't ask me why it does this!) DXP has some auto-routing and auto-placement functions, but I haven't found these to by particularly useful and have typically ended up doing the placement and routing by hand.

In general we use the top layer for components and the bottom layer for the traces, however the exact use of each layer can be set in IsoPro. The lab standard is ~10-20mils for signal traces and ~30-40mils for power lines. I've found down the line that it's easier to work on boards with larger traces and so I've pushed the size up a bit to ~30mils for signals. However when you do this, you need to take special care to ensure that the isolation goes as planned.

Rules

DXP allows the definition of a large number of design rules which will constrain the physical construction of the board. For example, DXP allows the definition of a "clearance" rule (Design->Rules;Electrical->Clearance->Clearance). By setting this rule to say, 31mils, you will be able to see when (by a change of color) components are closer than the clearance. By obeying this spacing constraint, there will not be problems during isolation with a 30 mil tool.

Note on Rules: The default maximum track width rule is 10mils. If you leave it at this, any track that is larger will turn green as an indication that you have violated the track width rule. If you want to be able to see when there is a problem, change the maximum width (Design->Rules;Routing->Width) to the maximum size that you want to use.

It is useful to use the "interactive routing tool"(p-t keyboard shortcut) if you started with a schematic. This tool will automatically respect the nets that have been defined on the schematic and will not allow you to place a trace if it violates, for example, the clearance rule.

Tips

• Define the board shape: Design->Board Shape -> Redefine Board Shape.
  • If you want to import the board shape into the CAM program, outline the board on the layer Mechanical1.
• Delete the Room that is generated every time the board is updated from the schematic. The Room automatically violated design rules.
• Use the interactive routing tool (p-t keyboard shortcut) This tool will respect the design rules and connectivity nets.
• When placing Vias associate the via with the relevant NET (press TAB).
• The ground and power nets can be turned off through View->Connections->Hide Nets and then by clicking on the nets to be hidden.
• Multiple components can be edited with the Inspect panel. This can be used in conjunction with the List panel and the use of selection filters.
• Polygon Fills can be made with the Polygon Plane tool. For use with Sierra ProtoExpress set the track width to 10mils and the Grid to 9mils. Set the Hatching style to Horizontal. The fill can be connected to a specific net (e.g. GND) by setting the Pour Over Net to the desired net.
• DO NOT USE POLYGON FILLS! (except when sending out for fab) Using a polygon fill to generate, for example, the top ground plane will result in a poor board which will take forever to mill. At the moment the best known technique is to simply delete the pads (top and bottom) for the ground net. This can be time consuming but the result is clean.

Exporting

The drill and Gerber files are exported from the File->Fabrication Outputs menu option. It is necessary to generate two types of files, NC Drill files and Gerber files, which must be exported in two different steps.

NC Drill Files

Select NC Drill Files from File->Fabrication Outputs. Note the Format and Leading/Trailing Zeros settings as these will have to be matched when Importing into CircuitCAM. This will generate a bunch of files and open a new window (a CAM file). We are only interested in the projectname.txt file which is output in the location specified in Project->Project Options->Options->Output Path. Feel free to delete the other files that are generated. (DXP will remove them from the project next time that you open it, don't worry about it.)

Gerber Files

Select Gerber Files from File->Fabrication Outputs. Select the layers that you want to export, typically Top Layer, Bottom Layer, and perhaps Mechanical1 if you have defined the board outline. DO NOT mirror at this point, it is much cleaner to do this in IsoPro. Ensure that the apertures are embedded under the Apertures tab. Again, this will output a ton of files, most of which aren't useful. The files that we are interested in have extensions .GBL .GTL and perhaps .GML which correspond to the bottom, top, and mechanical layers respectively.

A SPECIAL NOTE:

It is imperative that you NOT look at the '.gbl', '.gtl', and '.txt' files while you are still in DXP. If you do look at them, they will NOT be recognized properly, even if you do not modify them. Just don't look. Trust me. There's a measurement back-action that takes place, and you can't undo it.

CircuitCAM

Circuit CAM is used to prepare the DXP outputs for use on the circuit plotter. It performs the following functions:

• Isolation: Converting tracks into the outline path the cutter will follow
• Tool Asignment: Choosing the tools to use for drilling, milling, and routing
• Rubout: Removing all copper from certain areas of the board.

In addition, CircuitCAM can be used to define arbitrary additional copper regions on the board.

Importing

There are two options for importing, using the wizard or using File->Import. I prefer the latter and so will describe that procedure.

Begin by selecting File->Import. This will bring up a file selection window. Either select individual files or, using control, select all layers at once. The gerber files that are needed will have the extension .G*L with the * the initial of the relevant layer, and NC Drill file has .txt extension and the same base name as the gerber files. If you select multiple files to import at once note the order in which they are selected as the file name may not be visible when selecting the target layer.

Once the files are selected, it is necessary to assign a layer and parameters for each file. If you selected multiple files the import dialog will appear once for each file. The dialog seems to bring up the layers in the order in which they were selected, but preview is useful for determining exactly which file you are dealing with.

Gerber Files

All that has to be done is to select the correct layer for the file. The standard layers are Top Layer, Bottom Layer, and Board Outline (if the Mechanical1 Layer was used). Be aware that the default color scheme in CircuitCAM is defined in such a way that the top layer is colored red and is the one that will be mirrored. This usually corresponds to the component side of the board, while most traces will be on the bottom layer (colored green by default). Remembering this can help you avoid creating useless boards in which the mirroring is reversed.

NC Drill Files

The format and Leading/Trailing Zeros settings need to be matched to the settings that were used during the export from DXP. The preview dialog is useful to ensure that the correct settings are selected. I select the DrillPlated layer because this is drilled during the first half of the milling cycle before the board is flipped, but the DrillUnplated is technically correct.

Rubout Areas

Rubouts are used to remove all non-trace copper from a specific region. The procedure for creating a rubout differs considerably from the procedure in IsoPro. Rubouts are created by defining closed regions that will be rubbed out during isolation. Three standard layers are used, RuboutTop, RuboutBottom, and RuboutAllLayer. Other regions, such as the board outline can also be used to define rubouts. Selecting the layers to use for rubouts will be discussed in the section on isolation.

To create a rubout region:

• Select the relevant rubout layer from the lefthand drop-down menu on the top toolbar.
• Drawing a closed region with the tools on the left toolbar.

OR

• Click the rubout button on the bottommost top toolbar (circuit traces with the top half covered in a shaded rectangle) to draw a rectangular region in the RuboutAllLayer layer.

Isolation

Isolation is the process of converting the positive traces into inverted tool paths to remove copper surrounding the traces. Isolation can be performed by calling Edit->Insulate. This opens the Insulate dialog. The settings are described below. Once they have been set, press RUN. If you press OK the isolation will not be generated.

NOTE: Before proceeding, it is advisable to look at the section on tools to understand what tools are to be used in what circumstances.

Main Tab

• Select the desired job (top layer or bottom layer).
• Choose the tools to use. The standard is to use either the .2mm Universal cutter (8mil) or the 31mil end mill for the standard tool. If there will be rubouts, select a tool such as the .31mil or .39mil end mill as a Big tool if the standard tool is the .2mm cutter.
• Rubout Tracking direction can be used to make the rubout more efficient.
• Leave the Base and Special settings.

Advanced Tab

This tab is used to control the detailed behavior and to define relevant layers. Important settings here are:

• Rubout 1: Select a layer containing rubout regions for the layer being isolated. The Standard is RuboutTop or RuboutBottom, but could be, for example Board Outline to remove all extraneous copper.
• Rubout 2: A second rubout source layer. The standard to use is RuboutAllLayer.
• Remove Spikes: This option will round remove the sharp corners/shards that can be lead to shorts.

Routing

Routing is used to create define the outline of the board. If you have NOT imported an outline,

• create an outline of the board: Select the layer board outline from the drop down and draw the outline of the board.

With the outline defined, create the tool route:

• Edit->Contour Routing'
• Set:
  • Source Layer: Board Outline
  • Destination Layer: CuttingOutside
• Click RUN

Exporting for Board Master

• Open the Layers dialog (at the center of the left-hand toolbar)
  • Set only the layers that will be machined to visible and all other (used) layers to not visible. The layers to be machined are usually
    • InsulateTop_Std
    • InsulateBottom_Std
    • DrillPlated or DrillUnplated
    • CuttingOutside
    • and, if used, InsulateTop_Big and InsulateBottom_Big etc.
• 'File->Export->LPKF->LPKFBoardPlotter

Tips

• The layers menu is useful for working with specific sets of layers and hiding layers that aren't currently being edited.
• The drop down menus at the top can be used to control the tools that will be used. This is especially useful for choosing to use only a few standard drill sizes.

Board Master

Turn on the Plotter before starting Board Master

NOTE: On startup a dialog appears asking about the tool currently in the head (the "main clamp"). It is imperative that you set the dialog to the current status. If there is a tool in the clamp make sure to check in the main clamp and enter the empty tool location. The locations are numbered 1-10 from left to right. If the machine thinks that there is a tool in the clamp but there isn't, click the In the main clamp radio button to clear it.

Importing the CAM File and initial setup

File->Import->LMD

Note that the shaded region does not correspond to the actual dimensions of the board, so when placing the board be sure to check that it lies within the actual copper region. Board placement is accomplished using the move button (two squares linked by diagonal lines). The head of the unit can be positioned manually using the move to button (four arrows pointing outward) or using the manual step keys (four arrow buttons).

Tool Setup

Before milling it is necessary to ensure that the machine has the proper tools loaded into the tool holders.

• Open the tools dialog (button with three blue tools above a single tool with arrows showing a cycle)
• The tools that will be required for the milling process are shown in the top right of the window. The tools are labeled from left to right from 1 to 10.
• The tools that are required are listed at the TOP of each of the drop down menus, not in alphabetical order.
• Insert the needed tools and then return
• Note that the Universal Cutter(8mil) is the orange .029 universal milling tool

Milling

NOTE: If any point there is a problem with the machining, OPEN THE COVER TO STOP THE MACHINE IMMEDIATELY Pressing the stop button will not stop the machine immediately.

Board fabrication is broken into a series of phases. The phase is selected with the drop down menu at the bottom left of the tool bar. To mill a standard circuit:

• Select the first phase 1. Marking Drills
• Select the traces: to be machined-- press ALL +
• Begin Milling: Press the large Start button.
• Select the next phase, Drill Plated and repeat
• After the milling bottom phase the board must be turned over. Flip along the LONG axis.
• Continue through the Cutting Outside layer.

Additional Information

Tools

There are a number of tools available for the machine. Using the correct tool for the job will ensure longer tool life and a better finished product. In addition, it is critical that the tool depth be set properly.

We have the following tools for the machine:

• Drills: These tools have a green collar and are used for drilling holes...
• Universal Cutters: This tool has a conical tip and can be used to cut traces of varying widths based on the depth of the plunge. This is tool cuts fast and clean. The .2mm Universal Cutter(8mil) seems to be the machine's favorite tool. It is labeled in or set of tools as the Universal Milling Tool with .029 on the orange collar.
• End Mills: These tools cut square bottomed traces and the smaller ones are explicitly designed for RF work. The small ones also cut slowly. The smaller ones are not recommended for general use. The 31mil and 39mil end mills will cut quickly and are good for removing lots of material
• Contour Routers: These are used to mill through the entire width of the board. The Large holes, such as those for mounting screws, are automatically milled with the contour routers.
• Marking Drills: At the moment a universal cutter 8mil is used for marking the holes to be drilled.

Preparing Board

At the moment, the distance between the pins in the base is 11.6". Holes for the pins can be drilled with a #31 drill bit (.120").