QuickCAM Circuit Mill How To

From Qwiki

Jump to: navigation, search

This is an update to the lab QuickCircuit operating Howto for the current suite of design software. The typical design begins with schematic capture/PCB layout in DXP, followed by isolation and preparation in IsoPro, followed by circuit milling using QuickCAM and the QuickCircuit 5000 mill. (Note: The QuickCam functionality is built into the new version of IsoPro, and some of the below should be modified accordingly.)

Contents

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.

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.

If it isn't in our library, here are some hints:

  • The bundled PCB libraries are located in "Program Files->Altium->Libraries and non-specific libraries are in the PCB subdirectory.
  • The POT footprint matches the footprint of our POT's with in-line leads: matching the standard Bourns type 3296 footprint.
  • Not everything is in the libraries. It's pretty easy to define new components and footprints (by defining a new library) so you can add components. See the tutorial for an intro to this. We should put together a central lab library for when this happens... I'll work on it.
  • Surface mount component footprints are "0805" for standard caps, "1206" for standard resistors, and "SO-8" for standard Op-Amps.

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.

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.

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. The default settings should work. 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 and Bottom Layer. 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 and .GTL which correspond to the bottom and top 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, IsoPro will not recognize them properly, even if you do not modify them. Just don't look. Trust me. There's a measurement backaction that takes place, and you can't undo it.

IsoPro

IsoPro is a software package to convert raw layout files (Gerber, DXF etc) into files useable on the circuit mill. The conversion includes both formating (converting to the proprietary QuickCAM format) and inversion (isolation). Inversion is necessary because the circuit mill operates by removing material. A trace must therefore be converted to an outline to be made on the mill.

Loading Files Into IsoPro

  • create a new workspace
  • File->Import->Auto-Detect, select folder, select .gbl, .gtl, .txt. (Be sure to select them in the order stated above—that is, click on them in that order, so in the little file load-up box, they appear in the opposite order. This is just a bit of voodoo, necessary to insure that the drill marks are imported properly.) Click ‘Open’. A dialog box shows up. Pick the top option, which should be in English units.
  • Save As something.

Registering

  • The orientation of the board is defined by the open circle on the workspace which corresponds to front and center on the mill.
  • Be careful using the rollball on the mouse. If you accidentally use the rollerball, and can no longer find the circuit marks, use the home button next to magnifying glasses.
  • The layers should be registered on top of one another automatically, but if not:
    • elect all of one layer, press green/red register button, drag one layer to the other.
  • Translate the layout to the appropriate region of the board
    • Set all layers to Edit
    • Select everything with the cross
    • Move everything to the appropriate region with the offset button (the blue squares

Isolation

  • Set the layer types
    • Click the layers button (looks like a stack of colored sheets)
    • The trace side (generally gbl/bottom for axial components) should be set to solder and mirrored
    • The top side (gtl/top) should be set to component.
    • The drill layer .txt should be set to drill.
      • Since we typically have signal traces on the bottom layer and a ground plane on the top, it is most important that the bottom layer by cleanly registered to the drill holes. Thus, I will mirror the drill and bottom layers and make sure that I mill these first, since without the drill holes registering the opposing faces of the board would be impossible.
    • All the layers should be set up with default apertures.
  • Go toAperture Tabl and Drill Table, adjust numbers appropriately. Basically this step is here in order to adjust for any problems with the pads/wires/etc. thickness and shape which may have occurred due to problems importing the protel file. (e.g. the footprint for a surface mount device may not have the proper pad shape. You can correct this by making the pads ‘rectangles’ of the proper ‘width’ and ‘height’.) You probably won't need to do this if just using axial components.
  • Before isolating, delete any pads/shapes that you don’t want to isolate from the main copper area. For example, if a pin is to be soldered to the ground plane.
  • Isolate top and bottom layers: go to Tools->Isolate
    • Select component and solder layers and choose the tool size
      • When you pick the tool size, Isopro will isolate the components by drawing lines of thickness the ‘tool size’ around them. But, if some components are closer to one another than the ‘tool size’, isolation will not go well—Isopro won’t Isolate certain things because if you were to actually try to isolate this circuit with the chosen tool, you would end up cutting vital circuit track, component pads, etc.. So, for circuits with well-spaced leaded components, the .031” tool size is fine. However, for surface mount stuff, the .015” isolation is most reliable.
      • Make sure not tu use a tool that is larger than the tool that you specify, if you do it will kill your traces
    • Isolate
    • [Optional]:Rubout
      • If you wish to remove large areas of metal, create a rubout layer BEFORE EDITING THE ISOLATION LAYER AT ALL
      • Put the layer to be rubbed out on Edit and all other layers on something else
      • Select Tools->Rubout and pick the area to be rubbed out
    • Now, look carefully at the isolation layer and make sure that you have isolated everything that needs to be isolated. Pads that are particularly close together may not have been isolated. Use the drawing tools to draw on the desired isolation layer where needed.


Routing and Exporting

The penultimate step is to create the outline of the board:

  • Create a route data layer
    • Layers button, create new layer, name it, set type to contour, don't mirror it if you mirrored the drill layer (this is the last thing that you will mill, so make sure that it has the same mirror property as the second to last mill step...)
    • Draw a square around the circuit with only the new route layer on Edit
  • Create a names layer if you want to add text to the board. You can also just put this on a non-mirrored layer

Finally, export the files to the QuickCAM format. (Note: The user can mill directly from the new version of IsoPro and exporting to an independent QuickCAM program is not necessary.)

  • File->Export->QuickCAM
  • Select the layer to export and name it (.plt)
  • Repeat for the other files (4 total, drill/txt, top_isolated, bottom_isolated, route)
Retrieved from "http://qwiki.stanford.edu/wiki/QuickCAM_Circuit_Mill_How_To"