• Save frequently – you never know when your computer might crash
• Be sure to place connectors on your schematic for every input to or output from your board. These are located in the library “connector.cml”
• If you are in the ECE Computer Cluster, be sure to enable Technology Files before starting on your schematic:
  1. Go to Settings>>Preferences
  2. In the Preferences window, go to the General tab
  3. In the Folders section at the bottom of the window, click browse and navigate to "C:\Users\Public\Public Documents\DesignSpark PCB 7.1\Technology", then click "Ok"

Video Tutorials

DesignSpark New User Videos

DesignSpark PCB Tutorial Videos

Creating a New Part

Other Tutorials

DesignSpark Recommended Tutorials

Schematic

· Space bar to place a wire or component

· Press “R” to rotate a component

· Press ‘x’ or ‘y’ to place along the x or y axis, press again to disable. This prevents you from moving in the other axis, i.e. pressing ‘x’ only allows movement along the x axis.

· Scroll with middle mouse button to zoom in and out

· Middle mouse button (hold and drag): pan/move screen

· Labeling: Tools>Annotate Quietly or…

Tools>Annotate Schematic. ‘Update Changes List’, ‘Accept Changes’, ‘Execute Changes’

Then recompile project: Project >> Compile; then check for errors/warnings.

• Activating the Technology Files
  • You will need to do this if your schematic is yellow and red lines on a black background. This will typically happen on DesignSpark PCB on campus. Currently, you will have to do this every time you make a new design on campus. This issue is being worked on.
    1. Go to 'Settings'>>'Preferences'.
    2. In the 'General' tab, go to the bottom section labeled 'Tech Files' inside the 'Folders' section (if you do not see this section, you will have to switch computers).
    3. Click the 'Default' button or select 'Browse...' and go to 'C:\Users\Public\Documents\DesignSpark PCB 7.1\Technology', then press 'OK'
    4. Select 'Apply' then 'OK'
  • If you had already started a schematic/PCB you will have to make a new schematic/PCB. To save some time, you can select your entire circuit by clicking and dragging to select your entire circuit schematic, copying it (Ctrl+C or 'Edit'>>'Copy'), and then pasting it into your new schematic.

· To activate the built in libraries of DesignSpark PCB

· To open the Library Manager, go to File > Libraries (or enter Ctrl+L or select book icon)

· In the now open "Library Manager" window, click the "Folders" tab

· In "Folders and Search Order:", select the "*\DesignSpark PCB 7.1\Library" folder

§ If enabling libraries in the ECE PC Cluster: Click "Add" on the right side of the window. In the dialog box, enter "C:\Users\Public\Documents\DesignSpark PCB 7.1\Library" and press "OK". Repeat this for the folder "C:\Users\Public\Documents\DesignSpark PCB 7.1\Library\Default" as well.

· With the desired folder selected, check the "Folder Enabled" box on the right.

· Press "Apply" then “Close”

· Still can’t find desired parts?

1) Make a new component or 2) use a component with the same pinout and footprint (okay since not simulating) and make sure it is properly labeled in your schematic/PCB layout

PCB

· Space: place component or trace

· Alt + Backspace: undo

· While drawing a trace: right click and go to Segment Mode to change trace style

o Free – trace not constrained to any angles

o Orthogonal and Right-Angle – Trace restricted to right angles

o Mitre – Traces restricted to 45° angles, recommended

o Fillet – Traces curve, not recommended

· Shift+L: places via while routing (must have trace placed before placing via to continue)

· You might want to manually route what you want then autoroute the rest (autorouting more than once might create problems); check messages when done

· To move traces (first select the correct layer tab)

· Click and drag: Moves trace, keeping initial segment the same

· Click, release, click again: Moves trace, introduces angles

· Print each layer separately at 100% to see actual size of board/components/footprints/holes.

· Add text on silkscreen overlay by pressing ‘T’ or selecting the ‘A’ icon and choosing the ‘Top Silkscreen’ layer.

· DRC (design rule check): Tools > Design Rule Check; might see many errors here. Look for critical ones to fix. Some might just be that your silkscreen overlay text is under a component.

Resizing Traces

• Go to Settings>>Design Technology
• In the window that was just opened, go to the tab "Track Styles"
• If you are making your PCB here, ensure that all sizes are at least 25 mils/thous, otherwise ensure all track sizes are appropriate to your design/manufacturing specifications
• Click "Apply"
• If there are traces on your board, some may have changed size. This may require moving some of the traces to ensure proper spacing requirements for manufacturing.

Creating Copper Pour

1. Go to Add >> Copper Pour Area >> Rectangle (or Polygon if needed)
2. Draw the outline of your copper pour
3. Right click and select cancel to stop using the copper pour area tool
4. Select the outline of your copper pour area and right click it
5. Select "Pour Copper"
6. In the window that now opens, select which net this copper should be connected to, designate the finger width and isolation gap (minimum 20 thous), press "OK"

If you use the "Pour Copper" button on the toolbar on the left side of the DesignSpark window, it will fill all copper pour areas (top and bottom) and connect to the selected net. This would mean that both the top and bottom planes are ground, for example.

Enabling Board Outline for Export

1. Open the "Output Manufacturing Plots" window (Output >> Manufacturing Plots...)
2. At the top of this window, click the "Add Plot..." button
3. Press the "Gerber" button in the new window
4. Make sure this new plot is selected in the "Plots:" area of the window, and on the right side the "Output" tab is open
5. Rename the plot to something like "Outline" or "Board Outline" and change the "Plot Type:" field to "Outline"
6. Change tabs to the "Layers" tab and double click on "[Board Outline]"

You should now have an Outline Gerber file generated alongside the rest of your files.

Exporting Fabrication Files

1. Open the "Output Manufacturing Plots" window (Output >> Manufacturing Plots...)
2. On the left side on the "Plots:" field, select the layers you wish to generate by checking the check box. If you have a non-rectangular board outline, make sure to enable the Board Outline plot as above.
   1. For in house fabrication, you will need the Top Copper, Bottom Copper, Drill Data, and Board Outline (if you have a specific shape for your board)
   2. For out of house fabrication, check the vendor's website for details. Most will require Top and Bottom Copper, Top and Bottom Silkscreen, Top and Bottom Solder Mask, Board Outline, and Drill Data.
3. Ensure that all plots have the correct settings
   1. For in house fabrication, leave everything default except the Drill Data - [Through Hole] settings. With this layer selected, go to the output tab and click on the "Device Setup..." button. Under "Units..." set Integer to 2 and Decimal to 4.
   2. For out of house fabrication, check the vendor's website for details.
4. To set the Output Files export location, click the "Options..." button
5. Click the Run button

This will export the desired manufacturing plots to the location set in step 4. For in house fabrication (and most vendors), these files will need to be in a .ZIP file. To do this, navigate to where you output the files using the File Explorer and select all of the relevant files using Ctrl+leftclick. Then, right click the highlighted files, go down to "Send to..." and select "Compressed (zipped) folder" (or use your favorite compression software to compress them to a .zip archive).

Troubles Translating to PCB?

• Check if the components in your schematic all have footprints
  • You can do this by right clicking a component and selecting "Edit Component in Library...". This will open a new tab with the component symbol in the top right and the footprint in the bottom right. If the footprint is just an outline of a yellow box, your component does not have a footprint.
• Make sure all voltage and ground symbols in your schematic are from the "DesignSpark.cml" library.

Issues with Milling?

If you receive feedback about your drill file having an issue with decimal places:

1. Select Output --> Manufacturing Plots
2. Select Drill Data - [Through Hole]
3. Make sure you have the output tab selected within that window.
4. Click the "Device Setup..." button.
5. Under "Units"... Set Integer equal to 2. Set Decimal equal to 4.
6. Click the "Output in Metric Units (mm)"

Then create your manufacturing files as normal.

If you have questions or information you think would be helpful for this site, please email it to paul.rogers@ndsu.edu.