Hint

THIS DOCUMENT IS NOT PART OF MENTOR DOCUMENTATION!!

Hint

https://github.com/clalarco/pads-cheatsheet

Cheat Sheet for

• Start Schematics PADS Maker Schematic
• Start PCB PADS Maker Layout

Schematics

New Project

in ‘Start Page’ tab, select in ‘New Project’ pane > Design

Add a new Sheet

pg down on a active sheet

Change page size

1. Unselect all
2. In Properties, change Drawing size and orientation
3. In page, RClick > Change border… to select a proper border

Show Parts Panel

View > Parts

Parts

Add a part

1. Choose symbol from PADS Databook
2. drag and drop it into the page

With Nets

Check ‘Add Nets’

With names in Nets

Also Check ‘Add Net Names’

Add Ground, VDD, links, etc

Add > Special Components or

Hint

• Same part may have multiple symbols!
• If you put a part over a net, it will be automatically splitted!

Manipulation

Rotate

r or pick handle

Mirror Horizontally

h or m or

Flip Vertically

f or v or

Array

1. Select components
2. 
3. Set rows and column
4. Set spacing

Duplicate

1. Select part; then Ctrl+C, Ctrl+V, or
2. Select part, then Ctrl+LClick and drag LClick

Nets

Add a net

1. n or
2. LClick in start
3. Draw and LClick on end

Add nets to pins

1. n or
2. Alt+LClick on pin

Bus

Add

1. b or
2. LClick to draw
3. ESC
4. In Properties > Name, set NET_NAME[n:0]

Rip nets from bus

1. RClick on Bus > Rip Nets
2. Select nets (Ctrl = multi)
3. LClick

Connect a symbol to the bus

1. Touch bus with symbol pins
2. Select the bus indexes to connect and order
3. put symbol away from the bus to draw nets

Links

Setup

1. Setup > Settings
2. In Cross Probing, Check ‘Zoom Fit to Selected objects’
3. In Advanced, check ‘Automatically synchronize Links and net names’
4. Click OK

Add

1. In My Parts > Special Components > Link
2. Connect link to net
3. In properties, set a name for the link
4. Add another Link with the same net

Navigating

Alt+LClick over a Link.

Selection Filter

then select the elements to enable by selection

Add custom filters

Choose ‘settings…’ in combobox

Create a PCB from schematics

1. Tools > Prepare for Layout
2. ECO > Forward Annotation. Select filename.

PCB

Begin

1. Open PADS Maker Layout
2. Tasks > New > Select Layers Board
3. File > Import… and select .dnf file
4. Choose the proper footprints if required

Outline and keepouts

Set Board Outline and cutouts

>

Tip

RClick for polygon options

Edit outline

1. Clear selection
2. RClick > Select Board Outline
3. Pick outline trace and move

Add keepout

> and draw, then set parameters

Layers

Set Layers

Setup > Layer Definition

Change layers number

1. Click Modify
2. Set new number
3. Check reassignment

Pan and Zoom

Pan Up/Down

mouse wheel

Pan Left/Right

Shift+mouse wheel

Zoom

Ctrl+mouse wheel

Selection

Single

LClick

Region

LClick and drag

Add/Remove into selection

Ctrl+LClick into item

Visibility

Layers Colors

Ctrl+Alt+C

Hint

Items with background color are hidden

Nets Colors

1. Ctrl+Alt+N
2. Select net or class
3. Click ‘Add’
4. Set color and what to show
5. Check ‘color traces by net’ to show trace with the same color

Parts Placement

Disperse

Tools > Disperse Components

Move components

1. Pick part
2. Ctrl+E or LClick and drag

Rotate

Ctrl+R or tab

Change layer

Rclick > Flip Side or Ctrl+F

Rules

Open Dialog

Setup > Design Rules… and select scope:

Note

Scopes - Default Set rules for all nets - Net Set rules per net, overriding Default

Hint

• “Report” generates a report with rules

Note

Sections - Clearance Set trace widths and separations - Routing Set layers to route and via types

Set Trace Width

Clearance > Trace width

Set separation for different nets

Clearance > Clerance section

Set separation of objects for same net

Clearance > Same net Section

Allow Via at SMD

Clearance > Same net > Via/SMD set 0

Components separation

Clearance > Other > Body to Body

Drills separation

Clearance > Other > Drill to drill

Set allowed Layers

Routing > Layer biasing (selected = enabled)

Set allowed via types

Routing > Vias (selected = enabled)

Set maximum number of vias

Routing > maximum number of vias

Routing

Setup Dynamic Route and Bus Route

1. Tools > Options > Design
2. Set On-line DRC to Prevent

Begin

1. RClick > Select Pins/Traces/Unroutes

Start route

1. LClick over pin or trace
2. F3

Confirm a segment

LClick or space

Undo a segment

Backspace

Change Layer

F4 or l<n>

Autocomplete

Double LClick

Stop Routing

Ctrl+LClick

Change Width

w<width>

Add a via

Shift+LClick

Add testpoint

While routing RClick > Add testpoint

Add jumper

1. While routing RClick > Add jumper
2. Select orentation and length

Via at SMD

1. RClick > Select Traces/Pins
2. LClick on pad
3. RClick > Add Via at SMD

Hint

To enable via at SMD, via to pad distance for the same net should be zero.

Bus Route

1. Rclick > Select Pins/Vias/Tacks
2. Select pins to be routed together
3. RClick > Bus Route

Hint

If one of the traces in cannot be routed, it will ask you to route it separately.

Copper

Add

1. 
2. for solid copper or for copper pour or for plane shape only in mixed plane layers
3. Draw shape

Add cutout

1. 
2. for solid copper or for copper pour or for plane shape only in mixed plane layers

Edit

1. Clear selection
2. RClick > Select Board Outline
3. Pick polygon trace and edit

Tip

RCLick for polygon options

Vias

Note

• Pad stack The via shape in the layers
• Via Span The default via used to pass from one layer to another
• Through Via via crossing all layers
• Partial Via Via crossing a only some layers (blind and buried vias)

Setup

Set via Pad Stacks

1. In Layout () Setup > Pad Stacks
2. Set Pad Stack type to Via
3. Select Via and change properties

Add a via padstack

1. In Pad Stacks dialog, set Via type and Click in ‘Add Via’.
2. Select through or partial
3. Set start an end layer for partial vias
4. Set pad styles for Pad and thermal

Set default vias

1. Setup > Design Rules… > Default > Routing
2. At Vias section, select vias (selected = enabled)

Parts

Symbols

Hint

Use PADS Maker Schematic

New Symbol

In an existing design: File > New > Symbol

New Symbol (box type)

1. Create csv from template
2. In an existing design: File > New > Symbol from Pin List

Hint

Check wiki help “Creating and Editing Parts/Symbols”, Method #3 for excel template

Footprints

Hint

Use PADS Maker Layout

Add a Decal

1. Select decals section and partition
2. Over Partition RClick > New Decal…
3. If possible, use Decal Wizard

Use Decal Wizard

1. >
2. At bottom, select units
3. Choose type (dual, quad, polar, BGA/PGA)
4. Fill data, click OK.

PartQuest

Register

1. Go to http://partquest.com
2. At top-right, click on ‘Create Account’. It will redirect to mentor.com site.
3. Fill the form and click on ‘Create Account’
4. Once registered, log in
5. At top-right, click on your name, then click on ‘My Profile’
6. Check Desktop Integration. Select ‘Direct Download’
7. In Default flow, select ‘PADS Integrated’

Download parts

Download one part

1. Open PADS Maker Schematic and load a project
2. At checkboxes, check “Symbol/Footprint”
3. At search box, enter the name of the part
4. (Recommended) also check RoHS Complaint and Lead Free
5. Click on ‘More’ at the part from results
6. Check that no warnings appear
7. Click on Download. Select Partition if required.
8. Once the file is downloaded, double click on it.
9. On PADS Maker Schematics, the part will be immediately included into the library at PartQuestDirect partition.

Hint

You can use filters to reduce the search results

Download multiple parts

1. Follow the same steps than before, except instead click on ‘Download’ click on ‘Add to Project’. Select the project or create a new one.
2. When all parts are selected, at left pane click on ‘My Projects’ and select the project
3. Click on every row to download or in ‘Select All’
4. Click on ‘Download’ above the table headers.
5. Double click on the .pqz file to add the new parts into the library.