Best Practices in PCB Design: Finalizing for Fabrication in Ultiboard

Publish Date: Aug 01, 2017 | 8 Ratings | 2.62 out of 5 | Print | Submit your review


This document provides Ultiboard users with practical tips and recommendations on what to do when finalizing a PCB design fabrication. To ensure a quality PCB is returned back from a manufacturer, users need to ask:
  • What final steps should be taken to complete the design?
  • What must be done to check for errors?
  • How I completed all steps to successfully receive a completed prototype from a board house?

This document will discuss how to best work with the Ultiboard design rules and connectivity tools. Users will also learn how to setup necessary reference numbering, as well as final back annotation steps and manufacturing file generation.

This is the first in a series of articles that:
  1. Help you finalize for fabrication in Ultiboard
  2. Discuss exporting Gerber files for prototype fabrication

Table of Contents

  1. Final PCB Checks
  2. Design Rules Check
  3. Reference Designator
  4. Final Annotation Steps
  5. Next Steps

1. Final PCB Checks

It is an important first step in Ultiboard to perform standard PCB layout checks for routing completeness. Users can utilize the built-in diagnostic tools, specifically the DRC (Design Rules Check) and the Connectivity check.  

A final manual inspection of each layer is also recommended for thoroughness and a suggested manual procedure for performing these final visual routing checks is also outlined below. 


Back to Top

2. Design Rules Check

The Design Rules Check (DRC) is an automated tool in Ultiboard used to verify that the layout does not have any specific placement, routing or other addressable layout errors.  This operation will check the netlist and layout against the PCB design constraints and rules.  It checks the board’s part placement and routing integrity for overlapping components, untraced pins, incorrect layer placement and constraints that are set for trace width routing and clearances.  

Basic design constraints should be set prior to starting board layout but can be refined as the design is developed.   Be aware that changes after placement and routing may yield additional DRC errors that will need to be addressed. 

To initially set the PCB rules and constraints:

    • Select Option > PCB Properties (Figure 1)
    • According to the chart below, select the appropriate tab and apply the settings outlined in the table below

Figure 1 - PCB Properties


The table contains  generic considerations for each PCB specification settings and constraints for quick turn PCB services such as Sunstone Circuits. A quick turn PCB can be considered as being:

    1. 2,4,or 6 layers
    2. 0.062” board height
    3. 1 oz copper weight





Grid & Units

Grid Step Value

  1. Ultiboard Default: 15 or 20 mils.
  2. Recommended:  User Preference (1 or 5 mils)
  3. For more precise placement of copper, parts and vias - consider setting each Grid Step type to 1 mil.

Copper Layers

Board Outline Clearance

  1. Ultiboard Default: 10 mils
  2. Recommended: 20 mils or larger
  3. This will prevent inner copper layers from accidently being exposed.

Copper Layers

Board Thickness


  1. 0.062”
  2. This is usually the only size available for quick turn PCB services.


Pads/Vias(Vias Section)

Drill Diameter (Pad Diameter)


  1. Ultiboard Defaults: Drill: 20, Pad: 40
  2. Most quick turn PCB services will have only a few selectable options for drill sizes.  It is recommended to use the smallest drill size and pad size available for vias to closely space pads to signal connections.


Design Rules (Trace Width Setting)


Trace Width

  1. Ultiboard Default: 10 mils
  2. Recommended: 8 or 10 mils
  3. Quick turn PCB services will have a minimum trace width specification to follow.


Design Rules (Trace Width Setting)


Minimum Trace Width

  1. Ultiboard Default: Min: 0.039 mils
  2. Recommended: 6 mils typically recommended.
  3. See manufacturer’s recommendations on minimum trace width requirements (6 mils is common).


Design Rules(Clearances Settings)


Clearance to Traces


  1. Ultiboard Default: 10 mils
  2. Recommended: 10 mils
  3. Minimum clearances are given by the PCB manufacturer.

Design Rules(Clearances Settings)


Clearance to Pads

  1. Ultiboard Default: 10 mils
  2. Recommended: 10 mils
  3. Minimum clearances are given by the PCB manufacturer.

Design Rules(Clearances Settings)


Clearance to Vias

  1. Ultiboard Default: 10 mils
  2. Recommended: 10 mils
  3. Minimum clearances are given by the PCB manufacturer.

Design Rules(Clearances Settings)


Clearance to Copper Areas

  1. Ultiboard Default: 10 mils
  2. Recommended: 12 mils (or higher if pwr/gnd planes used)
  3. Minimum clearances are given by the PCB and can be safely be obtained on both top and bottom layers, however Inner Layers (such as ground planes) may have special restrictions based on drilled hole sizes as holes may be plated in quick turn PCB services (see below).




There are typically size restrictions on the holes and for quick turn services only selected sizes may be available.  The manufacturer will usually default hole sizes other than specified to one of the available fixed



Back to Top

3. Reference Designator

Reference designator renumbering is a process for renaming the reference designators from top to bottom, left to right on the PCB so that it is easier to locate parts on the boards during assembly, test and troubleshooting.   If reference designators are left numbered as is locating specific parts on larger designs will be time consuming and difficult.

To renumber the parts in a left to right, top to bottom fashion (when either top or bottom sides of the board is viewed from a face up perspective) follow the procedure below:

  1. Select only top side parts first.  To select only top side parts, first make Copper Bottom and Silkscreen Bottom invisible (see Design Toolbox - Figure 2 below in which both Copper Bottom and Sikscreen Bottom are unchecked)

Figure 2 - Design Toolbox


  1. In the Select toolbox, set  the Enable Selecting Parts filter (deactive all other filter elements).


Figure 3 -Select Toolbox


  1. Drawing a rectangle on the design area to select all the visible top layer parts.
  2. Select Tools -> Renumber Parts… (Figure 4)
  3. Select the Ok button.

Figure 4 - Renumber Parts


This procedure will renumber the parts from left to right on the top side of the board.

  1. Next renumber the bottom side parts.  Re-enable the bottom side layers and then deselect Copper Top and Silkscreen Top layers.
  2. Select the visible bottom side parts. 
  3. Select Tools -> Renumber Parts…
  4. In the Start Corner drop-down box select Lower Left.
  5. Click on the Ok button.

Now that the parts have been renumbered, it is time to back annotate the new reference designators to the schematic so the reference designators will match between schematic and layout.  A new BOM needs to be generated.


Back to Top

4. Final Annotation Steps

Annotation is the transfer of design changes from schematic to layout, or layout to schematic.  After performing any change in Ultiboard that modifies reference designators, footprint shapes or net names, it is recommended to perform a back annotation step to synchronize the schematic with the layout design.

Refer to for more details about annotation.

What can be forward annotated? (Multisim to Ultiboard):

    1. Standard schematic changes (net renaming or reassigned net-pin assignments)
    2. Reference designator changes originated from Multisim
    3. Footprint changes originated from Multisim
    4. Trace width and other constraints

What can be back annotated? (Ultiboard to Multisim):

    1. A change in the part Reference Designators (Part renumbering)
    2. A changed footprint (component is removed in Multisim and needs to be manually replaced)
    3. A deleted footprint

What cannot be back annotated? (Ultiboard to Multisim):

    1. Components added to the design
    2. A modified net connection between components
    3. A pin and/or gate swap


Important Note

In order to safeguard any work it is always recommended to backup the layout file prior to a forward or back annotation.  The files can become out of sync in cases where changes were made to both schematic and layout.



After making changes in Ultiboard (such as renumbering parts), the Backward Annotation can be started by following these steps:

  1. Go to Multisim and select Transfer > Backannotate from Ultiboard… (Figure 5)
  2. Select the ‘filename.log’ where filename matches the Ultiboard project filename.
  3. Select Open.
  4. An annotation log will be displayed that shows all of the pending changes.
  5. Select OK to invoke the changes.
  6. A text file of the back annotation log will be shown confirming the changes.
  7. Close the text file window.
  8. In the case of renumber parts, the schematic now has the new reference designators that match the layout.
  9. Save the files in Multisim and Ultiboard.
  10. Create a new Bill of Materials report in Multisim.  This will reflect the new reference designators.  After exporting to a spreadsheet, the data can be used for ordering the parts as well as creating a kitting list for production.


Figure 5 - Backannotate


Tip: After renumbering footprints it is a good practice to check the reference designator locations and rotation orientation so the refdes text can be easily found and seen for component population, rework or testing.  If the refdes text will be obscured by a pin or the component body it is best moved to a more visible location.  When moving, the refdes will show a line connecting back to the part so there is no confusion as to which part it is associated.


Back to Top

5. Next Steps

Now that you have finalized your design it is time to:

  1. Export files for fabrication: Exporting Gerber Files

View these articles to learn more about the final steps of the prototyping process.


Back to Top

Bookmark & Share


Rate this document

Answered Your Question?
Yes No