Multisim Tools for Making Custom PCBs

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).
  • Basic Circuit Design
    For this workshop it is assumed you have basic experience with Multisim. That said, the skills necessary for this workshop can be acquired quickly, as Multisim is used only for layout, and a knowledge of simulation tools will not be necessary. These are skills that should get developed in regular course work.

 

  • Concepts of Nets
    A "net" is another term for a connection or a "virtual wire." In terms of circuit theory, a net is a "node". By default nets are the red lines connecting component terminals according to your design

    To make net numbers visible, right click on a blank part of the schematic, then click properties. In the Sheet visibility tab, under "Net names" click "Show all." Nets will be auto-assigned a number name, however a descriptive name can be given to the net by right clicking it > Properties > Enter in the name under "Preferred net name." Something to note below is that though V1 and R5 are not connected with a red line, they are both connected to ground, which Multisim will automatically assume is the same net.

    A part of a schematic showing labeled net connections
    A part of a schematic showing labeled net connections

     

    • Net Properties (and how they translate to PCB)
      At the bottom of Multisim's window is a section called "Spreadsheet View" and at the very bottom are some tabs (Results, Nets, Components, etc). Click Nets to view Net Properties.
      The 'Nets' tab of Multisim
      The 'Nets' tab of Multisim

       
      Typically, when you are doing simulations in Multisim, the net properties are not too important. But once you start designing a PCB, these properties become very important. In this tab, you can change the following properties of your selected net (only relevant properties are mentioned):

      • Trace width: This will specify the width of the trace in mil (Note 1 mil is 1/1000 inch) A larger trace width can handle a larger current
      • Trace length min and max: These specify the limits of the lengths that a trace can extend. Typically you shouldn't have to enter any value in these cells, unless you are dealing with a very special noise sensitive signal where you want carefully control the electromagnetic properties (IE if the trace is acting as an antenna)
      • Trace to Trace: This specifies the "Volt Spacing" between traces. This specifies the physical distance (in mil) between the selected trace and any other trace. Note that if the specified spacing for two parallel traces varies, Ultiboard will always use the larger value.
      • Trace to pad: This value specifies the volt spacing between the trace and any given solder pad. As a rule of thumb, I would say it's safe to keep trace spacing the same for all spacing properties (IE Trace to Trace = Trace to Pad) UNLESS the board will not be coated with solder resist. Then it is a good idea to increase the spacing from Trace to pads to prevent accidental solder bridges. The upper and lower limits can also be specified.
      • Trace to Via: Specifies the spacing between the trace and any given via. It's typically safe to keep this the same as the Trace to Trace spacing value.
      • Trace to copper area: Specifies the distance between the trace and any given copper area (copper plane typically used for power distribution)
      • Routing Layer: PCBs can consist of multiple layers. By default, Multisim will set the design to a two layer board. To increase the amount of layers, click (at the top of the window) Options > Sheet Properties > PCB and then increase the "layer pairs" number. Which layer you choose to route signals on is entirely up to you. A standard is to keep small signals on a separate layer from power signals.

 

  • Types of components and circuits (Simulated, layout only, etc)
    There are three types of circuit components you can add in Multisim their type specifies their function in Simulation and PCB design.
    • Simulation and layout (model and footprint): These components can be used in your Multisim simulations because they have a SPICE code assigned to them. They can also be used in the PCB layout because they have (or will have) a footprint assigned to them. These components are colored blue.
    • Simulation only (model): These components only have SPICE code, and no footprint. The components will not show up on the PCB design in Ultiboard. These components are colored black.
    • Layout only (footprint): These components to not effect the simulation and are only used in PCB design. These components are colored green.
      An image demonstrating the three types of components
      An image demonstrating the three types of components

 

  • Making custom components
    The sad truth about Multisim is it doesn't have every electronic part that has ever been created. So, sometimes, you have to create a model of the component yourself! This is typically a 6 step process that starts by clicking (at the top of the window) Tools > Component Wizard.
    • The first screen is the "Component Information Screen" page. Here is where you name the component that you are creating, summarize its function, and select the component type. Typically, you're going to be selecting "Layout only" unless you have an intimate understanding of the part and are interested in including a SPICE model as well. I'm not going to go over that though. Click Next.
      Component Wizard - Component Information Screen
      Component Wizard - Component Information Screen
    • The "Footprint Info" screen is where you will select the footprint for your component. If the component is a standard form factor, you can click "Select a footprint" > Master Database where you'll have to do some searching to find the exact form factor you are looking for. If you've already created a footprint it will be in the "Select a footprint" screen under "User Database." If you plan to make a new footprint but haven't made it yet, just type in the name of the footprint in "Footprint type", specify the number of pins on the component, and then click next. It will ask you to fill out some information about the footprint, which should be strait-forward. If you are dealing with a component with a lot of pins, consider clicking the "Multi-section component" dot, in order to split the layout representation into multiple pieces.
      Component Wizard - Enter Footprint Information Screen
      Component Wizard - Enter Footprint Information Screen
    • The "Symbol information" screen is where you can review the schematical symbol that Multisim generated for your part. You can edit it to any shape that might make more sense for your schematical layout. Note that changing this symbol will not change anything on the PCB layout.
      Component Wizard - Enter Symbol Information Screen
      Component Wizard - Enter Symbol Information Screen
    • The "Pin Parameter" page will allow you to name pins, select which section the pin is include in (if you selected the symbol to be multi-section in the previous step), the signal type, and the ERC Status (If it its connections are checked by the error checker). I typically keep the Type and ERC status at the default settings.
      Component Wizard - Set pin parameters screen
      Component Wizard - Set pin parameters screen
    • The "Pin Mapping Screen" is where you connect the assign the schematic pins to the footprint pins. Do so by clicking the "Map Pins" button. It is sometimes safe to click the "Auto Assign" button if your symbol pin names are numeric values starting at 1. But in any other case (IE you named the pins alpha-numeric names) you are going to have to manually assign pins to one another)
      Component Wizard - Pin Mapping Screen
      Component Wizard Pin Mapping Screen
    • The last step in the "Family Tree Selection" screen is where you can either select a family in the user data base or corporate database to save you designed component. The corporate database is for parts that might be hosted on a company server that multiple people would use.
      Component Wizard - Family Tree Selection Screen
      Component Wizard - Family Tree Selection Screen
  • Transferring designs to Ultiboard
    There are two tasks you might want to accomplish when designing transferring a design to Ultiboard.
    • A New Design: If the design is new, at the top of the window click Transfer > Transfer to Ultiboard > Transfer to Ultiboard 13.0. This will prompt you to create new files that will open up in Ultiboard
    • Changing an Existing Design: If you make a change to the schematic, but already have a PCB design in progress, you are going to have to "Forward Annotate". To do this, click Transfer > Forward Annotate to Ultiboard > Forward Annotate to Ultiboard 13.0. You can save the net list at a revision, and then select which board file you would like to revise.