Academic Company Events NI Developer Zone Support Solutions Products & Services Contact NI MyNI
What is Developer Zone?
United States

Document Type: Tutorial
NI Supported: Yes
Publish Date: Mar 04, 2009


Feedback


Yes No

Related Categories

Products

Development Topic

Industry

Application Type

Technology

Related Links - Developer Zone

Related Links -Products and Services

NI Ultiboard Prototyping: Sunstone Circuits Prototyping Check List

1 Ratings | 5.00 out of 5
 Print |  PDF

Overview

This article is a new design resource for all engineers who are looking to prototype their custom designs using NI Ultiboard, and the Sunstone Circuits fabrication house. Sunstone Circuits are a member in the National Instruments Circuit Design Ecosystem. By working with us they can provide order integration to ensure that designs are quickly put through the order process.

Written by engineers who have extensive experience in prototyping, along with the co-operation of Sunstone Circuits, this is a valuable resource for all prototyping their circuits.

In this document you will find a checklist of settings for you to consult when creating a prototype which will be fabricated by Sunstone Cirucits. You can download a word document checklist at the bottom of this article.

This is the third in a series of articles that:

  1. Help you finalize for fabrication in Ultiboard
  2. Discuss exporting Gerber files for prototype fabrication
  3. Provide a step-by-step check-list before prototype fabrication

Table of Contents

  1. Pre-Layout Checklist
  2. Post Layout Checklist
  3. Exporting to Sunstone Circuits

Pre-Layout Checklist

General Checks

The following is a checklist of settings for you to consult when creating a prototype which will be fabricated by Sunstone Cirucits. Sunstone Circuits are a key element of the National Instruments Circuit Design Ecosystem. By working with us they can provide order integration to ensure that designs are quickly put through the order process. 

This checklist has been defined as an aid for those prototyping their circuits in Ultiboard at Sunstone Circuits. This is for those designs that have the following characteristics:

  1. 2,4 or 6 layer quickturn designs with silkscreen
  2. Board height of 0.062"
  3. 23/24 style pre-defined holes
  4. 35 holes/square inch
  5. Copper weight: 1oz

 

PCB Properties

To set the following values:

  1. Open Ultiboard (Start > All Programs > National Instruments > Circuit Design Suite 10.1 > Ultiboard 10.1)
  2. Create your new layout
  3. Select Options > PCB Properties

Now with the checklist, ensure that you have the following settings:

 

Checklist

Tab

Section

Setting 

 

Grids & Units

Grid Step Values
  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. Min: 20 mils
  2. Recommended: 25 mils (not UB default)

 

Copper Layers

Board Thickness

 
  1. 0.062”

 

Pads/Vias

(Vias Section)

Via Drill  / Pad Diameter

 
  1. Min Drill: 16 mils / Pad: 31 mils
  2. Recommended: Use Min Settings (not UB default)
  3. Max Drill: 20 mils / 40 mils

 

Design Rules

(Trace Width Setting)

 

Trace Width

 
  1. Recommended: 8 or 10 mils (10 is UB default)
  2. Max: 100 mils

 

Design Rules

(Trace Width Setting)

 

Minimum Trace Width

 
  1. Min: 6 mils (not UB default)

 

Design Rules

(Clearances Settings)

 

Clearance to Traces

 
  1. Min: 6 mils
  2. Recommended: 10 mils (UB default)

 

Design Rules

(Clearances Settings)

 

Clearance to Pads

 
  1. Min: 6 mils
  2. Recommended: 10 mils (UB default)

 

Design Rules

(Clearances Settings)

 

Clearance to Vias

 
  1. Min: 6 mils
  2. Recommended: 10 mils (UB default)
  3. See special notes about Inner Layer drill spacing below*

 

Design Rules

(Clearances Settings)

 

Clearance to Copper Areas

 
  1. Min: 6 mils
  2. Recommended: 12 mils (not UB default)
  3. See special notes about Inner Layer drill spacing*

 

Other Setting Considerations

 

Hole Sizes

 
  1. Ultiboard: No default
  2. Sunstone uses 23 hole styles from 0.16” to 0.251” for manufacturing (0.08” holes are available on 4, 6 layer services).  Any holes will be mapped to the available default hole sizes other than specified to one of the available fixed sizes.  Most through- holes will be ok, however if a precise hole is required consult the website and choose a specific hole size (or next size up) for the desired hole.

Inner Layer Clearances*
  1. Ultiboard: 10 mils default (12 mils recommend for inner planes)
  2. Increase clearances on any ground or power planes on the inner layers if large holes over 0.100” are present.  Individual planes can be set with a specific clearance setting.

 

 

Post Layout Checklist

General Checks

Perform the following standard checks on your file (generally done prior to the export process):

Checklist

Setting 

Check

 

Netlist and DRC
  1. Correct any issues found

 

Connectivity
  1. Complete any traces

 

Visual Checks
  1. Check net names
  2. Check power (Verify IC connects to power source and ground)
  3. Use net preview (in spreadsheet view) or print out individual layers

 

Trace Widths / Clearances
  1. Verify traced widths: 6 mil minimum
  2. Verify trace clearances: 6 mil minimum
  3. Verify plane clearances: 12 mil minimum or more for inner layers

 

Hole Checks
  1. Confirm holes min/max: 0.016” to 0.251” (0.008” on 4/6 layers)
  2. Hole spacing should be 10 mils min. edge to edge
  3. Hole density: 35 / square inch maximum

 

 

Gerber and NC File Generation

Gerber File Generation

In Ultiboard you can export a number of different industry standard formats including Gerber files. Sunstone Circuits accepts the Gerber RS-274x standard.

To export in Ultiboard:

  1. Select File > Export
  2. Select RS-274x
  3. Click on the Properties button

Ensure that your export has the following properties:

 

Checklist

Export 

Setting 

 

Gerber Style
  1. Gerber RS-274X

 

Gerber Layers
  1. Select Board Outline, Copper Top, Copper Bottom and all Copper Inner layers.
  2. Select Solder Mask Top and Solder Mask Bottom
  3. Select Silkscreen Top (and Silkscreen Bottom if any parts on bottom)

 

Board Outline
  1. Merge Board Outline Layer and Copper Top Layer

 

Soldermask 
  1. Check the Oversize Soldermask options for both Solder Mask Top and Solder Mask Bottom.  Set each to 8 mils.

 

Export
  1. Click on Ok to set settings, and then choose Export to save all layers to multiple files

 

NC Drill File Generation

To export in Ultiboard:

  1. Select File > Export
  2. Select NC Drill
  3. Click on the Properties button

 

Checklist

Export

Setting

 

NC Drill
  1.  Verify imperical units as default, choose Export to save .drl and .rep files

 

Prepare Exported Data

 

Checklist

Action

 

Rename Files

Remove project name from the Gerber files.  For example, “AmpProf – Copper Bottom.gbr” should be renamed to just “Copper Bottom.gbr”

 

Create zip File

Zip all .gbr, .drl and .rep files and rename zip file to the project name (or part number/revision number)

 

 

 

Exporting to Sunstone Circuits

Step 1: You can begin your export process from Sunstone Circuits by beginning at the ni.com/multisim web-page. View the Sunstone Circuits third-party page at http://www.ni.com/multisim/network/sunstone.htm.

 

Step 2: Click on the Order from Sunstone link.

 

 

Step 3: Enter the information based upon your board design.

 

Downloads

8570_sunstone_checklist.doc

1 Ratings | 5.00 out of 5
 Print |  PDF

Reader Comments | Submit a comment »

 

Legal
This tutorial (this "tutorial") was developed by National Instruments ("NI"). Although technical support of this tutorial may be made available by National Instruments, the content in this tutorial may not be completely tested and verified, and NI does not guarantee its quality in any way or that NI will continue to support this content with each new revision of related products and drivers. THIS TUTORIAL IS PROVIDED "AS IS" WITHOUT WARRANTY OF ANY KIND AND SUBJECT TO CERTAIN RESTRICTIONS AS MORE SPECIFICALLY SET FORTH IN NI.COM'S TERMS OF USE (http://ni.com/legal/termsofuse/unitedstates/us/).