HobECAD Tutorial

As a final comment, you are welcome and encouraged to store additional project information into these directories. For example, if you are using a microcontroller, the source code for your microcontroller should live in the same directory. Likewise, any documentation or specifications can also be stored there. In addition, I tend to do all of my projects so that they can be viewed via the web, so all of my HTML (HyperText Markup Language) files live in the same directory structure. Since none of these files are directly related to learning HobECAD, they have been omitted from this tutorial.

Now it is time to enter a schematic for the digital logic probe.

Creating a Schematic

Before starting the schematic, it is useful to have a short discussion of "Why?" There are three important reasons for doing a schematic. First, it provides a human readable diagram of the circuit. Second, it is possible to get HobECAD to verify that the printed circuit board exactly matches the schematic(s). Thus, when you are debugging the circuit, there is high confidence that the schematic actually matches the circuit you are debugging. The third reason is because HobECAD can do a little signal checking to verify things like there is no short between ground and Vcc and the like.

In addition to helping you create the circuit schematic, the hobecad program reads the circuit schematic(s) and generates a wire list that describes which leads of what components are attached to one another. In addition, The hobecad program can also read the printed circuit board and extract a wire list. Since both lists are generated in alphabetical order, the standard Unix style diff program can high light the differences between the two wire lists. When there are no differences between the two lists, the user has high confidence that the printed circuit board implements the schematic(s).

Now that I have explained why you should have a schematic, it is time to actually use hobecad to create one. The project I have selected is an inexpensive digital logic probe. Please follow the following steps:

1. Start hobecad as follows:

   	prompt$ hobecad -c 10 myproject.sc
   								

   The -c 10 tells HobECAD to use 10 pixel square cells. The .sc tells HobECAD to go into schematic capture mode.
2. After you start hobecad, you are presented with a white window with a small black square in the lower left corner. That small black square is the cursor. The cursor can be moved by clicking on the left mouse button over the location you want to move the cursor to. The cursor color can be toggled between black and brown by clicking on the middle mouse button. Lastly, the thickness of the cursor can be changed by clicking on the right button. Please experiment a little by clicking on all three buttons. Do not worry if you accidently draw any lines.
3. To exit without saving anything, click on the the little `X' on the top most row of the window. Please do so, right now. Please note that it immediately exits without giving you a chance to change your mind. It typically displays an error message of the form:

   	X connection to :0.0 broken (explicit kill or server shutdown).
   								

   This message is OK; please do not worry about it. When you click on the `X', editing immediately terminates, any edits you have done are lost forever, and they can not be recovered. (No, this is not considered to be good user interface design, but it is what hobecad does.)
4. If you do a directory listing, there will be no file named proble.sc because you exicted without saving.

   	prompt$ ls
   	{directory listing here}
   								

5. Let's restart hobecad:

   	prompt$ hobecad -c 10 probe.sc
   								

   Again, we are presented with a blank white windows with a black square in the lower left corner. We are back to where we stared. Cool.
6. Now this time, let's exit hobecad and save the file contents. This is done by depressing the [Esc] key (typically in the upper left hand side of the keyboard.) Please depress the [Esc} key now. Notice that the window disappears and there is no confusing message from the window system. If you do a directory listing, you will find that the file probe.sc now exits.
7. You now know how to start editing with hobecad and two ways of leaving hobecad ([Esc] and `X'.)
8. Now it is time to do some actual editing. Restart hobecad on probe.sc:

   	prompt$ hobecad probe.sc
   								

   You will note that this time the -c 10 option is not specified. This is because the file remembers its cell size when it written out. It may be tempting to try to edit schematics at a different cell size, but frankly there are too many bugs for that to work; so please do all schematics at a cell size of 10.
9. Now we are going to enter some text. Please click the middle mouse button to change the cursor color to brown and type the following:

   	Copyright (c) 2002 by First M. Last
   								

   where First M. Last is your first name, middle initial, and last name. (Actually, nobody really cares what name you use, so you can be creative here.) As you type in each letter it, the cursor advances one cell to the right. Upper case letters are bold and lower case letters are shown as non-bold upper case letters. There is a good case the text does not fit in the square window. You can resize the window by grabbing any corner with the left mouse button and resizing the window. Now using the mouse, position the cursor above the first line (use left mouse button), change the cursor color (use middle mouse button) to brown, and type:

   	Digital Logic Probe (Rev. A)
   								

   The resulting screen should look as shown below:

   

   with the exception of the mark in the upper right and corner (please ignore the artifact for now; it is just a way to trick the software into drawing the window at a reasonable size.) If the characters are black, you should delete them (see next paragraph) and switch them over to brown.
10. When typing in text, you can use the [Del] key to delete the character to the left of the cursor. Indeed you can insert charcters into the middle of the string using the mouse to click the cursor to the desired insertion point. Likewise, you can delete characters in the middle of the string. For example, replace your middle initial with your full middle name and delete the characters back.
11. You now know how to insert and delete characters. It is always a good idea to but some information on the schematic that specifies what it is (i.e. a digital logic probe), what revision (i.e. revision A), when it was edited (i.e. 2002), who the creator is (i.e. you), and some sort of copyright notice. This information is completely optional in the sense that hobecad will process the file irrespective of whether or not the information is present or not; however it is still a good idea enter the information.
12. Now it is time to explain the purpose of the colors. With exactly one exception that is dicussed shortly, anything in brown is completely ignored by hobecad when it is reading your schematics. Anything entered in black is used by hobecad when it processing the schematic.
13. The subject of glyphs is introduced next. A glyph is basically an electronic symbol that has been preentered into the HobECAD symbol library. The various glyphs in the HobECAD glyph library can be found in the HobECAD documentation.
14. We are going to draw an operation amplifier (i.e. an opamp) into our schematic in the brown layer. Please move the cursor to approximately the center of the drawing area using the mouse, make sure the cursor is brown, and then type (in lower case):

    	opamp
    								

    the resulting screen should look as follows:

    

15. Now, with the cursor sitting somewhere on the word opamp, depress the [Control-X] key. This key code is generated by holding down one of the keys on the keyboard labeld [Control] or [Cntrl] and then depressing the [X] key while still holding the [Control] key down. There is no need to touch the [Shift] key. When you do this, an operational amplifier symbol shows up pointing down. It should look as follows:

    

    Notice that the text that spelled out opamp has been removed.
16. The [Control-X] key is used to insert a glyph into the drawing. It is done by typing the name of the glyph followed by typing the [Control-X] key. As far as HobECAD is concerned, the glyph is located where the first character of the glyph name used to be. There is no visible locator for the glyph location other than the glyph itself.
17. The [Control-D] key is used to delete a glyph. This is done by placing the cursor over exactly the glyph is located and typing [Control-D]. This causes the glyph to be deleted and we are back we we started.
18. Each glyph can be oriented in one of four directions - left, up, right, and down. If you just type in the glyph name, you get the down orientation. If you follow the glyph name with the character '<', '^', or '>', you get the left, up, and down orientations of the glyph. Please type in:

    	opamp>
    								

    followed by typing [Control-X]. You should wind up with the operation amplifier symbol pointing to the right as shown below:

    

19. You now know how to insert and delete glyphs using hobecad.
20. Next, we will learn how to draw lines. By the way, there isn't much more to the hobecad editor other text, glyphs, and lines.
21. Lines are drawn and erased using the mouse. A line is started by clicking the with left mouse where you want to start the line. Next, leaving the left mouse button depressed, the mouse is dragged to where the end point of the line is to be. hobecad will only draw lines that are vertical, horizontal, or at a 45-degree diagonal. Lines are erased by retracing the line.
22. Using the thin brown cursor, please draw a box around the operational amplifiere along with lines for the inputs, outputs, and power supplies. It should look as shown below:

    

23. Now we are going add a bunch of labels. The labels will identify the pin numbers for a common LM741 operational amplifier. We add labels inside of the box for the inverting (-) and non-inverting inputs (+) as well as the positive and negative power supply leads (V+) and (V-). These labels are done in brown. The pin numbers are done outside of the box in black (use the middle mouse button to change colors.) The user label for the op amp (U1) is done in black inside of the brown box.
24. In HobECAD schematics, a brown box is with a single black label is the only time where brown is recognized as part of the schematic. This is a component box, and the black label is the component label. The black numbers outside of the box are the component leads and they can be numbers, letters, or other characters such as plus (+) or minus (-).

    

25. Now we are going to draw our first wires in black now. Black lines represent always represent signal wires. Please add some black wires that look as follows:

    

    Whenever a black wire terminates on the side of brown box, hobecad looks for a black label that identifies which lead is being connected to. hobecad will get confused if it sees no black label or two black labels and will generate an error message when the wire list is extracted.
26. We need to indicate where two wires connect by adding a connection dot. This is done using the mouse. Place the black cursor over the connection point, depress and hold down the left mouse button, now click the middle button and a black connection dot will appear. To erase the connection dot, just do the same operation again. Your schematic should look as follows:

    

27. Now it is time to add a couple of light emitting diodes and couple of resistors. The resistor glyph is called resistor and the diode glyph is called diode. The glyphs are entered in black at the approximte locations shown below:

    

    And after you type [Control-X] over each piece of text, you get the following:

    

    And after some black wires and connections have been added and some brown diagonal lines to indicate light emitting diodes you should have the following:

    

    The black labels identify the components and for resistors and the diodes, hobecad "knows" what the leads are named. For resistors, the leads are named "A" and "B" and for diodes they are named "+" and "-". Lastly, the "100K" and "220" specify the resistor value in ohms in brown.
28. We are on the final stretch now. Let's add the 1.25 volt regulator (the LM317), the input probe (N1), and the voltage input terminals (N2). The resulting diagram should look as follows:

    

Parts Management

I need to give a few definitions here before we can get into the parts managment topic very deeply.

Component/Part

A component or part is an electronic part that performs a particular function -- e.g. a resistor, a capacitor, a transistor, a diode, an integrated circuit, etc.

Package

A package is the way a component is packaged up use in an electronic circuit. Many different components use the same package. For example, many integrated circuits come in the DIP-14 (Dual Inline Package - 14 pins.) Some components are alternatively in a TO-220 or a TO-92 package.

Lead

A lead is one wire connected to package. It can be used for signals or power. A DIP-14 has 14 leads, a TO-220 has 3 leads, etc.

Parts List/Bill of Materials

A parts list assigns a short name to each part used by a given board.

The purpose of parts management is to keep HobECAD informed about about the relationship between the parts list, schematic, and printed circuit board layout. The symbols in a schematic identify parts in the parts list. The printed circuit board layout needs to know about where the various leads of a component on a board are located. Eventually, HobECAD can scan through a parts list, and generate a corresponding list of vendors, part numbers and costs.

When designing HobECAD, I could not come up with a particularly compelling reason create a fancy graphical user interface for managing parts information. Instead, everything is kept in flat ASCII text files. Yeah, it is boring, but it is fairly simple to learn and manage. There are three file formats:

Parts List (.ptl)

The parts list makes an association between a symbol name on the schematic (e.g. N1, Q2, R3, U4, SW1, etc.) and a part (e.g. 74LS00, LM741, NE555, PN2222, etc.) Optionally, a suggested vendor and part number can be provided. A parts list file and schematic should be enough for somebody who is really dedicated to duplicate a circuit. This is exactly one parts list file per printed circuit board.

Part/Component Catalog (.prt

A component catalog list a bunch of parts that can be used in a project. Each entry specifies the component name, (e.g. 74LS00) the corresponding package that the omponent uses (e.g. DIP14), and a list of leads used in the package. (The lead list is discussed in greater detail later.) In addition, it is possible to optionally specify what a vendor, vendor part number, and vendor pricing information. More than one vendor may be listed in a single part/component catalog. In addition, multiple catalogs can referenced by a single printed circuit board design.

Package Catalog (.pkg)

A package catalog lists a bunch of different package names and the corresponding placement of the pins on a printed circuit board. Each entry consists of a package name (e.g. TIP31) and a list of leads. Each lead has a name (e.g. E, +, 1) and an X Y position relative to one pin which is designated as the pivot pin that the package can be turned about.

    # Digital Logic Probe (Revision A):
    #
    D1-2: LSG2040 - Green LED [Jameco: 34606]
    N1: Probe_Wire - Probe wire
    N2: Terminal2.Probe - 2 Junction Terminal Strip [Jameco: 189675]
    R1: 100K_Resistor - 100K Ohm 1/4 Watt resistor [Jameco: 29997]
    R2: 47_Resistor - 47 Ohm 1/4 Watt resistor [Jameco: 31106]
    U1: LM741 - Operational Amplifier [Jameco: 24539]
    U2: LM317LZ - Positive Voltage Regulator [Jameco: 23552]
								

    # Digital Logic Probe Part Catalog:
    #

    H Parts 1 0

    P LSG2040 LED1 - Green LED [Jameco:34606;LEDs $.15/10 $.13/100]
    L + + Other
    L - - Other

    P Probe_Wire Wire - Probe wire
    L 1 1 Other

    P Terminal2.Probe TerminalStrip2 - 2 Junction Terminal Strip [Jameco:189675;Connectors $.69/1 $.62/10]
    L 1 1 Other
    L 2 2 Other

    P 100K_Resistor Resistor4 - 100K 1/4 Ohm Resistor [Jameco:29997;Resistors $.99/100]
    L A A Other
    L B B Other

    P 47_Resistor Resistor4 - 47 1/4 Ohm Resistor [Jameco:31106;Resistors $.99/100]
    L A A Other
    L B B Other

    P LM741 DIP8 - Operation Amplifier [Jameco:24539;ICs $.29/1 $.25/10]
    L 1 OFFSET_NULL1 Other
    L 2 V- Other
    L 3 V+ Other
    L 4 GND Other
    L 5 VOUT Other
    L 6 OFFSET_NULL2 Other
    L 7 VCC Other
    L 8 NC No_Connection

    P LM317LZ TO92 - Low voltage regulator [Jameco: 25532;ICs $.49/1 $.39/10]
    L 1 VIN Other
    L 2 VADJ Other
    L 3 VOUT Other
								

    H Parts 1 0
								

    P 100K_Resistor Resistor4 - 100K 1/4 Ohm Resistor [Jameco:29997;Resistors $.99/100]
								

  # Digital Logic Probe Packages:

  H Packages 1 0

  P Wire - A wire for probe tip
  L 0 0 1*

  P TerminalStrip2 - 2 Junction Terminal Strip with .2" between leads
  L 0 0 1*
  L 0 4 2

  P LED1 - LED with .1" between leads
  L 0 0 +*
  L 0 2 -

  P Resistor4 - Resistor with .4" between leads
  L 0 0 A*
  L 0 6 B

  P TO92 - TO92 3 lead package splayed into a "V" with pin 2 pointing down
  L 0 2 1
  L 1 0 2*
  L 2 2 3

								

  H Packages 1 0
								

    make
								

  hobecad -C -w probe_sc.wl probe.sc probe.ptl ../probe.prt ../probe.pkg
								

    D1:+ D2:- U1:2 U1:6
    D1:- D2:+ R2:B
    N1:1 R1:B U1:3
    N2:1 U1:7 U2:1
    N2:2 U1:4 U2:2
    R1:A R2:A U2:3