Ultiboard Basics

Error message

Deprecated function: The each() function is deprecated. This message will be suppressed on further calls in book_prev() (line 775 of /home/voltfoli/public_html/main/modules/book/book.module).
  • The Rat's Nest
    The first thing you'll see when you transfer a Multisim design to Ultiboard is a bunch of components connected by a "ratsnest." The ratsnest are a bunch of thin yellow lines connecting components. The purpose of these lines are to signify that a trace has not yet been routed between the two terminals. Note that these connections are only virtual, and do not represent hard-wired connections on the PCB. You can turn off the ratsnest by unchecking it in the "Design Toolbox" at the left of the screen.
    Unplaced components connected by a Ratsnest
    Unplaced components connected by a Ratsnest


  • Setting Net Properties
    • Trace Width Calculation
      Trace width specifies how wide a trace is, which in turn specifies the maximum safe current capacity. The standards can be found on IPC-2221 (PCB Design Standards Document), and the equation can be derived from their given curves (Credit to 4PCB.com)
      Where k = 0.024, b = 0.44 and c = 0.725 for internal layers. For external layers: k = 0.048, b = 0.44, c = 0.725. Current given in Amps, Temp rise in Deg C, Thickness in Oz.
      • Parallel layers
        If for any reason you cannot make a trace wide enough (perhaps you can't make if fit between component pins), consider using using parallel traces of equal width, to effectively double current capacity. These parallel traces don't have to be on the same layer either.
      • Copper Thickness Availability
        PCBs can be made with varying copper thicknesses. Using a thicker copper will allow for a smaller trace width. However there are two things that you have to note when using non-standard copper thicknesses. First, does the manufacturer you intend to use supply that thickness? The second thing to consider is; As Thickness increases, the machinablity decreases. This means that traces will have to be wider (in order for it to be possible to manufacture), and volt spacing may need to be bigger. To determine if this is an issue and how to remedy it, you're going to need to call your PCB manufacturer and ask what their capabilities are.
      • How to use tools to calculate
        To be honest, I don't use the trace width equation given above. I'm efficient (no I am not lazy), and I use a tool called PCB Toolkit by Saturn PCB. When you first open the toolkit, there is a lot to digest. At the top, click "Conductor Properties" and take a deep breath. The top left section, and the right section is all input for the program, and the bottom left set of boxes are outputs. I'm going to discuss what I think is meaningful for this workshop. The rest are a bit technical, and with a bit of Googling, you can figure them out.
        • Plane Present?: If you have a whole layer that is mostly copper parallel to your trace, click "Yes" in this section. This will increase the allowable current through the trace. The reason is because you have a sheet of copper close to your trace that can act as a heat sink, which provides more surface area for heat dissipation.
        • Parallel Conductors: See the above section on parallel conductors for reasons on why you would want to do this. Note that the toolkit will only provide results for 1 of the conductors. So for example, if you have 2 parallel conductors and need to handle 1A, adjust your conductor width until the current is 0.5A
        • Conductor Width: Here is the main thing you want to work with. Vary this number until you have achieved the desired results in the bottom section.
        • PCB Thickness: A Standard overall PCB thickness is 62 mil. You're going to have to check with your manufacturer to see what the "Stackup" or thickness of your PCB is. When in doubt for a 2 layer board, typically leave it 62 mil.
        • Base Copper Weight: Copper Weight actually refers to the thickness of the copper. When it's time to get your board manufactured, you'll specify this. Copper weight relates to Copper thickness by the following equation
          $$Thickness(mil) = Weight (Oz) * 1.37$$
        • Conductor Layer: If your conductor is in an internal layer (for example if you have a 4 layer board)  then specify it as such. You'll notice that the conductor current will drop in comparison to the External Layer alternative. That is because there is now a layer of Epoxy glass insulating the trace, and heat cannot dissipate as easily as if it were on the top of the board exposed directly to air flow. Therefore it is a good idea to put high power traces on top or bottom layers
        • Temp Rise: I typically leave this value alone. This specifies how hot the trace can get above ambient before it melts (or you consider it to be too hot)
        • Conductor Current: This is how much current the trace can support with out heating up to a temperature above the specified Temp Rise.
        • Conductor DC Resistance: This indicates the resistance of the trace. Note that this is also highly dependent on Conductor Length. If a trace is already routed in Ultiboard, the length can be found in the "net properties tab"
        • Power Dissipation: At peak current, this is how much power will be dissipated by the trace.
          The PCB Toolkit Conductor Properties Tab
          The PCB Toolkit Conductor Properties Tab
    • Volt Spacing
      Volt Spacing (called trace clearance in Ultiboard) is a parameter that specifies the distance between the edge of a trace and another conductor. It is called "Volt Spacing" because this distance must be big enough such that there will not be possible for an electrical arc while at the standard operating voltage.
      • Researching manufacturer stack ups
        If you are concerned with volt spacing, you must also take considerations for multi-layer boards. Not only do you need to consider the spacing between traces on the left and right of a given trace, but you must also consider the spacing the trace and traces on top of, or below it. You'll have to contact the PCB manufacturer in order to find out what these distances are.
      • Also consider capacitive coupling
        Having conductors parallel to one another for a significant length (>5in) can cause a capacitive coupling effect. This will in essence make a low pass filter, and if the frequencies of the signals are high, they will be attenuated. Therefore it is a good idea to always minimize the amount of parallel conductors, and also keep as much space between conductors as possible.
      • How to use tools to calculate
        In the PCB Toolkit, go to the "Conductor Spacing" tab. Here you can select the voltage range you expect between conductors, as well as where the trace is located on the board (reference he provided key in the software for what B1, B2, etc. stand for). Note that B1's minimum spacing values are always smaller than B2. This is because it is harder to have an electrical arc travel through epoxy glass than it is for the arc to travel trough air.
    • Differential, or noise sensitive traces
      Noise sensitive traces can get very complex quickly. There are a lot of crazy techniques to "shield traces" or prevent noise from getting into the signal. Here are my tips to handling Noise sensitive traces.
      • Use differential analog inputs to get rid of common mode noise.
      • Keep the two signal traces very close together. That way any noise present will be induced on both traces. Since the signals are differential, the noise will be canceled out.
      • Keep your noise sensitive traces far away from any power traces, or anything that is switching. These traces cause a lot of noise, so it's best to be on the other side of the board from them.
    • All Net properties should be set before start of design
      This is important. Make sure you set all of your net properties before you start routing. If you complete routing, and then change properties of the nets, you run the risk of causing a lot of Design Rule Check errors (DRC) (IE if you change a trace width and it now overlaps another trace)


  • Footprint Design
    Designing custom part footprints can be very tedious if they are not a standard pin package. You can start this process by clicking (at the top of the window) Tools > Part Wizard. Below is an explanation of what's going on in each of the 7 steps for the wizard.
    • Technology
      Here's where you select what type of mounting the part is. Like all of the parameters in footprint design, this information will be found in the part's data sheet.
      The Technology Page of the Part Wizard
      The Technology Page of the Part Wizard
    • Package Type
      This step allows you to select some standard package types. The package type of your part should be specified in the data sheet. If you are making a footprint for a part that does not use any of the predefined package types, pick something close to use as a baseline.
      The Package Type Page of the Part Wizard
      The Package Type Page of the Part Wizard
    • Package Dimensions
      This specifies the dimensions of your part. Once again, reference the data sheet to find out this information. It is always good to use the dot for signifying pin 1 on your part. Though 3D data is needed for your board, it might be useful to visualize air flow across your board, or when/if you export the board design to a 3D file for mechanical engineering packaging.
      The Package Dimensions Page of the Part Wizard
      The Package Dimensions Page of the Part Wizard
    • 3D Color Settings
      Set the colors of your part to make your rendered 3D model look more accurate.
      The 3D Color Settings Page of the Part Wizard
      The 3D Color Settings Page of the Part Wizard
    • Pad Type and Dimensions
      Typically the only thing you should have to change here is the drill hole diameter (From your datasheet).  It's a good idea to keep the pad size as "Use design rules" unless you are having some sort of routing issues and need the pads to be smaller. If you have a part that has multiple different pin sizes, pick the most predominant size here, and we'll add/modify pins later.
      The Pad Type and Dimensions Page of the Part Wizard
      The Pad Type and Dimensions Page of the Part Wizard
    • Pins
      Here is where you set the number of pins on your part. Also set your distances between pins according to the data sheet. If you are using a non-standard package, just set your pin count, and then leave everything at default; we'll change it later.
      The Pins Page of the Part Wizard
      The Pins Page of the Part Wizard
    • Pad Numbering
      Name/Number your pins here. If you can't do it how you want in the Part Wizard, you can change pin numbers later manually.
      The Pad Numbering Page of the Part Wizard
      The Pad Numbering Page of the Part Wizard
    • Modifying Footprints:
      After you've finished with the Part Wizard, your screen will show your designed part. If you're happy with the way it looks, go ahead and save it (File > Save). If you have to make changes, reference some of the following pieces of advice.
      • Changing Pad Properties/Position:
        Right click a pad, and then select "Properties." In the Attributes tab, you can change the pin number. In the General tab, you can change the position of the pad relative to the origin point. This can be useful for fine tuning a pad's location. Also note that you can move the origin to a new point by Design > Set Reference Point. By moving the reference point, you can change a position relative to another pad. The Pad Tab allows you to change the physical dimensions of the selected pad.
      • Grid Spacing:
        You can adjust the grid spacing by clicking Options > PCB Properties > Grid & units. You can adjust the grid step value to make it easy to organize and lay out pads. For example if you have a segment of pins that is spaced 250mil relative to a pin, then set your origin to that pin, and then set your Grid step value to 250mil. It can also be useful to set the value to 0.0000001 to have virtually continuous placement options
      • 3D Data:
        You can turn on the 3D-Info Layer in the Design toolbox, and either edit the existing shape, or add shapes from Place > Shapes.


  • 3D Data and Transfer to Solidworks
    Once and awhile, you might need to include your PCB in a 3D model (Perhaps for designing an enclosure, or some other packaging purpose. To export the 3D model, click File > Export > 3D DXF. Note: when you import it, make sure you set the units correctly.


  • Planes
    Planes are large areas of copper that are left after the traces have been cut into the board.
    • Detrimental if left unconnected
      If a plane is left unconnected you might get capacitance-related issues. This is because these planes can build up charges, and not have any way to drain the charge. So always consider having a plane connected to a pin (IE Ground)
    • Can make routing easier
      A very common practice is to connect planes to power distribution pins. For example 5 volts on the top plane, and common on the bottom plane. This can be done by clicking Place > Power Plane. Then select which net you want, and which layer to route the net on.


  • Considerations on Board rigidity
    When designing boards, you should consider how rigid the final product will be. If you have a multi layer board, and you have planes cut out of a common area, you run the risk of the board flexing at that point. Therefore it is a good idea to use planes on every layer. Or at least use planes on the top and bottom layers.


  • Part Placement
    When placing parts, it can be useful to adjust the grid spacing, as well move the origin, to position in an organized fashion (See the above section on modifying footprints). Another useful group of tools is Edit > Align. In this menu, there are multiple options to align selected parts, and distribute them equally.


  • Routing
    • Line tool and its uses
      The Line tool can draw a trace anywhere. If you scroll over the end of an existing trace, you can continue drawing from that point. Be careful: The line tool will allow you to draw on top of existing traces, causing DRC errors. You must also use the line tool to connect to a newly place via.
      The Line tool Button
      The Line tool Button
    • Follow me tool and its uses
      The follow me tool will only connect a point on a net to another point on the net. This tool will not allow you to place traces that will cause DRC errors. When routing traces with this tool on long boards, it is best to place point by point in order for optimal placement. Ultiboard's automatic trace placement can be a bit messy.
      The Follow Me tool Button
      The Follow me tool Button
    • Via Placement
      Vias are used to connect a trace on one layer to a trace on another layer. You can place a via by clicking the Via tool in the top menu. Once you've placed the via, a "Select Lamination for Via" menu will pop up. Always select Copper Top and Copper Bottom, unless you are dealing with some special micro-vias. Keep in mind that each via an through-hole on your board is going to increase manufacturing costs. So it is a good idea to keep the via count to a minimum
      The Via Placement tool Button
      The Via Placement tool Button
    • Routing Logic
      • Ever other layer every other direction principle
        It is a good idea to route every other layer predominantly in opposing directions. This is for two reasons. The first reason is to minimize capacitive coupling, or in other words, having closely parallel traces. The second reason is it will make it easier when it comes to using vias and traces to cross over existing traces.
        The left two traces are placed to minimize cross over (Good). The right two traces have a lot of cross over (Bad)
        An example of good and bad trace placement
      • Differential pair routing
        Here is some information copied from the above section "Trace Properties"
        • Keep the two signal traces very close together. That way any noise present will be induced on both traces. Since the signals are differential, the noise will be canceled out.
        • Keep your noise sensitive traces far away from any power traces, or anything that is switching. These traces cause a lot of noise, so it's best to be on the other side of the board from them.
      • Keep to a side idea
        I realize this is contradictory to what was said earlier about keeping distance between traces, but it is also easier for routing if you keep traces tightly clustered. Doing this will give you more open areas to place vias where necessary.
        Traces routed tightly together
        Traces routed tightly together
      • Types of corners
        • 90 degrees and its detriments
          Ultiboard makes it difficult to place 90º angles for a reason. If 90º corners are avoided, traces will be shorter, and therefore resistances and inductances will be lessened. Also 90º traces can be hard to manufacture if using a mill.
          A right angle trace (bad) and a chamfered trace (good)
          A right angle trace (bad) and a chamfered trace (good)
        • Avoiding sloppy routing (minimize trace vertices)
          Another good practice is to reduce the amount of bends in a trace. The more bends in a trace, the likely a manufacturing error is. Also the board will look better aesthetically if things are kept simple.
          A poorly routed trace vs an efficiently routed trace
          A poorly routed trace vs an efficiently routed trace
      • Copy and pasting routing
        When doing a large circuit that contains duplicate sub-circuits, it can be useful to copy and paste routing and placement. To do this you must first either create a part group or net group bu going to Tools > Group Editor. Place and route the group in the desired configuration. Then select the next parts that you want to be placed in the same fashion. Make a group of these parts, and be sure that in the list, parts from the new group are in the same order as the old group. Then go to Design > Group Replica Place or Design > Copy Route.
    • The Autorouter
      It is possible to forgo all routing efforts by clicking Autoroute > Start/resume Autorouter. In simple boards this process should occur pretty quickly. Go through all the traces and clean them up, because I guarantee that there are unneeded bends. In order to use Autorouting well, it is assumed that you have all of the Net Properties set up correctly. Also be sure to set every other layer to be perpendicular at Options > PCB Properties > Copper Layers > Copper Layer Properties. For complex boards, the Autorouter will take a long time, and sometimes may not converge on a solution. This does not mean the board is impossible to make, it only signifies that a human touch (and logic) is required to make the remaining connections.
      I don't use the autorouter, because I feel that I can do a much better job logically routing traces. Don't let robots take your jobs, people.


  • Design Rule Check (DRC)
    While designing a PCB, it is inevitable for you to run into DRC errors. The most common errors you will run into are traces being to close to one another, vias being to close to something, something not connected, or something is incorrectly connected. These are represented by little red circles on the board design. You can go to each individual error by Clicking (at the bottom) DRC, and then click an error to go to that spot on the board. To recheck for errors, click Design > DRC and Netlist Check. If your board is left with erros when you send it out


  • Net List editor
    Sometimes it is nessisary to add components or connections on the Ultiboard file. This can be done by entering Tools > Netlist Editor. Nets can be added, renamed, and connections can be added in this menu.
    The Netlist Editor
    The Netlist Editor


  • Finalizing designs
    Congratulations. You've finished your design and are ready to send it out to a manufacturer. PCB manufacturers make your boards from Gerber files, not Ultiboard files. To create Gerber files, go to File > Export. I typically generate a gerber file for every option, however a manufacturer may not require all of them. Talk to your manufacturer and ask them what they require, but note that they typically won't mind if you send them more than they need (And they'll be sure to let you know if you didn't send enough). It is also typically a good idea to oversize your soldermasks by at least 1 mil. This will make your boards easier to solder to.
    The File Export Window
    The File Export Window


  • Revisions
    It may be nessisary to make changes to your design. If you've generated a forward annotation file by making changes in Multisim, go to Ultiboard, and click Transfer > Forward annotate from file. If you are making change to a board file and want to send the changes to Multisim, click Transfer > Backwards annotate to Multisim > Backward annotate to Multisim 13.0