Microsoft Word - CADSTAR 8.0 Express DIY Booklet v4.doc

• Contents:

• Introduction to CADSTAR

• The Basic Design Flow

• Design A

−

Step 1 - Schematic for Design A

−

Step 2 - PCB Placement for Design A

− Step 3 - PCB Routing for Design A

− Step 4 - Manufacturing Data for Design A

• Design B

−

Step 1 - Schematic for Design B

−

Step 2 - PCB Placement for Design B

−

Step 3 - PCB Routing for Design B

−

Step 4 - Manufacturing Data for Design B

• Design C (for advanced users, based on P.R.Editor XR)

−

Step 1 - Schematic for Design C

−

Step 2 - PCB Placement for Design C

− Step 3 - PCB Routing for Design C

− Step 4 - Manufacturing Data for Design C

• Design D (single sided board design for advanced users, based on P.R.Editor XR)

−

Step 1 - Schematic for Design D

−

Step 2 - PCB Placement for Design D

−

Step 3 - PCB Routing for Design D (adding Jumpers on the fly)

−

Step 4 - Manufacturing Data for Design D

• Conclusion

For more information visit www.cadstarworld.com

• Introduction to CADSTAR

Let me introduce CADSTAR to you. CADSTAR is a PCB Design tool allowing you to draw a Schematic
Design and transfer the Design to a PCB Layout environment. After an error-free transfer, CADSTAR
helps to place the components into the board outline.

Routing is an integral part of a PCB design process, and manual, semi-auto and automatic routing
tools are available within the Embedded Route Editor, or P.R.Editor XR (Place & Route Editor) in
CADSTAR. CADSTAR introduced the Embedded Route Editor for users who don’t use a PCB Design
tool regularly, and P.R.Editor for more advanced users, who require more powerful solutions. For more
advanced users (industry users), also high-speed design features can be provided as standard or
optional.

The completion of the PCB design will be followed by the generation of manufacturing output data for
PCB fabrication.

I will guide you through the basic design flow of a PCB design and through two very simple PCB
designs using CADSTAR. Try them and have fun!

• The Basic Design Flow

Library

Make sure that all the parts (schematic symbol & PCB footprint) required are available in
library.

Note:

the library provided with CADSTAR Express contains only a few parts essential

for the two PCB designs described in this 'Do-It-Yourself Book' and some examples of
the on-line CADSTAR Exchange Library. More libraries are available on-line through

CADSTAR Exchange

. The ready-to-download-and-use parts contain all the information

you require including manufacturers' part numbers. The libraries currently contain over

140,000 parts

and are updated and expanded regularly. If the part required is not

already available in these libraries, you can quickly and easily design your own parts
using the supplied wizards and the Graphical Library Editor.
The on-line CADSTAR Exchange Library is available to you as part of the maintenance
contract.

Schematic

It is always advisable to start with a schematic design before moving onto the PCB the

PCB

design.

PCB

After the successful transfer from schematic, components will be placed within the

(Placement)

board outline.

PCB

After placing all the components, we can start routing the critical nets manually and/or

(Routing)

through

automatic routing.

Manufactu-

The final stage of any PCB design. No matter what your manufacturer requires,

ring Output

CADSTAR can deliver Gerber, Ncdrill, Placement data, Bill Off Materials, IPC-D-356

test data, DXF, CADIF, GENCAD and ODB++

For more information visit www.cadstarworld.com

• Design A

Introduction to LED Flasher

This is a a-stable multi-vibrator circuit to
alternately flash 2 LEDs. The Resistor
and the Capacitor values determine the
frequency, which is the flash rate. The
formula is as follows:

LED Flasher

The design drawn has two 39 kOhm resistors and 10uF capacitors. However, the two sides do not
have to match. Different values for R and C on each side can give a nice effect for a unique duty-
cycle. The Flash-rate for this circuit is about 1 cycle per second.
The 470 Ohm collector load resistor limits the current flow to ~20mA and also determines the
brightness of the LEDs. 270 or 330 Ohm is recommended for green LEDs. Transistor in this design is
not critical.

Step 1 - Schematic for Design A

You shall start with going through the hand drawn schematic shown on the previous page. The
design is a simple LED flasher.

You will then have to gather the components being used in the flasher.

From the hand-drawn schematic, you should be able to see twelve (12) components, they are:

- 2 x 2N3904 NPN Transistor

- 2 x 1N914 Diode

- 2 x LED HLMP-1585

- 2 x 470 Ohm Resistor

- 2 x 39 kOhm Resistor

- 2 x 10uF/10V Electrolytic Capacitor

You can also see a 9V power supply. You can use a 9V battery for this power supply.

Once this information is available, you can start the CADSTAR Design Editor

Click on the Tool Bar (File New Schematic Design) and choose one of the templates- in the

box (I like Form A1)

[Time Off = 0.7 x R x C] R in ohms and C in farads
[Total Time Off = 1 / Frequency] Total Time Off being the total number of seconds that both
transistors are off and Frequency is in hertz.
[Time Half = Total Time Off / 2]
[Capacitor = Time Half / ( 0.7 * R )] with Capacitor answer in farads.

For more information visit www.cadstarworld.com

If you don't like to work with a black background, you can also select in the toolbar a

You can now start calling out the symbols you require by using the Workspace on the left of the

window. Click the Libraries Tab

You can start to place 2 transistors onto the schematic template by using the Workspace and

search on

and choose 2N3904

Place 2 transistors on the template by simply dragging the transistor from the Workspace
window, i.e. highlight 2N3904, click on it by using left-hand mouse button, without releasing the
button - drag it out onto the design template. While dragging, you can use the right-hand mouse
button for mirror and/or rotation.

Do the same for the other 10 components (you can either select the through-hole or SMD
components):

-2x Diode>1N914 (or BAS19)

-2x

Led>HLMP-1585

-2x Resistor>470E-MRS25-1% (or 470E-r0805-2%)

-2x Resistor>39K-MRS25-1% (or 39K-r0805-2%)

-2x E-Capacitor>10uF-10V-EC (or 10uF-10V-c6032)

While selecting the appropriate components in the Workspace window --> Libraries (like
2N3904), you can click on the right-hand mouse button to see Links --> Datasheet.

The link is a hyperlink to an URL on the internet (or

intranet), but can also be linked to something different (i.e. PDF file or Word document).

You can connect two components simply by placing the connecting terminals onto each other.

After you have added all the components, you can add 3 AGNDs. To do so, simply click the

Add --> Global Signal Icon

and choose (AGND). You can connect the AGND terminal and

the terminal of the diode (cathode), by placing the terminals onto each other.

After 3 AGNDs have been added, search on soldereye-1mm

and add 2 pins. The purpose of these 2 pins is the wiring connection to the Battery pads; hence
a pad is connected as 9V and the other AGND.

Change the pin names to VCC9V and AGND respectively. To change the name, select the pins

and click the Item Properties

icon.

Connect the symbols together in the same way as the hand-drawn schematic is connected

electrically. To connect, click the Add --> Connection

Icon. While connecting, you can also

use the right-hand mouse button to Change Default Net Route Code, allowing you to select a
different Net Route Code (I like Power & GND thicker than signal tracks).

Change the net name connected to VCC9V to VCC by selecting the net

and clicking the

Item Properties

icon.

When completed, save this schematic design

CADSTAR Express allows you to make pin names or numbers visible/invisible so you can see
which pin is number 1 or 2. Select Tools

Options

Display from the menu and

enable/disable Override Part Pin Names/Numbers Visibility.

For more information visit www.cadstarworld.com

In today's market it is important to deliver a B.O.M. (Bill Off Material, or in CADSTAR called
Parts List) at an early stage. To create a Parts List, simply click on Tools --> Reports --> Parts
List.

To print your schematic design, simply click on File --> Print Icon

and go through the Print

and Page Setup. Alternative if you have the Acrobat PDFwriter installed you can print your
schematic design to a

PDF

file.

Note: Enable Alternative text output in the print options, making text

searchable

when printing

to a file format such as

PDF

Finally, transfer the schematic to PCB through File --> Transfer to PCB, choose '

2 layer

1.6mm.pcb'

as PCB Technology.

Note: If you choose the PCB Technology '1 layer 1.6mm.pcb' during transfer to PCB, this
default technology file is prepared for single sided boards (whereas I prefer larger solder-pads,
thicker track-widths and more spacing). The advantage of the different technology files is that
you still can make use of ONE library as you will experience in Design D.

If you didn't complete the schematic design as described above, just open

Example1.scm

and

transfer the schematic to PCB through File --> Transfer to PCB, choose '2 layer 1.6mm.pcb' as
PCB technology.

Step 1 showed how a schematic design can be drawn for Design A. In fact, any schematic capture can
be drawn following the sequence shown. However, a more complicated design will require more
complicated steps. There are many tools within CADSTAR Design Editor that will help designers like
you to design a schematic. You can also add spacing classes, insert a component into a net without
any disconnection, auto-connection of busses. Other tools like Align Symbol, Design Re-use, Design
Variant, Hierarchical Design, etc are both important and user friendly for professional Design
Engineers. You can try them out!

Error free transfer, no netlist is necessary! CADSTAR Library, Schematic and PCB run on the same
Graphical User Interface, guaranteeing a fast & problem free transfer.

You can now move on to PCB Design.

Step 2 - PCB Placement for Design A

You are now in the PCB Layout area with all the 12 components and 2 pins stacked onto each
other.

You should make sure that the unit is Thou (Thousandth of an Inch / Mil) by Setting --> Units or
by double-clicking the units

at the bottom of the CADSTAR window.

First, you will have to draw a PCB outline; this board outline can either be drawn within
CADSTAR or imported via DXF format (File --> Import --> Format --> DXF). Select the DXF file
Boardoutline.dxf.
For the mapping-file, you have to select dxfio.map, which you can find in the User directory and
just click OK. If you succeeded to import the board outline, then go to step g.

Alternatively you can draw the board outline manually. Click the Shape

Default icon

and select Board. Then click any of the drawing tool

icons

and begin drawing a rectangular outline (size

2000x1000 thou). Watch the absolute and incremental coordinates at
the bottom of the CADSTAR window when drawing the board outline.
From any point in the design you can reset the incremental coordinates
by pressing the 'Z' key, followed by the return command.

For more information visit www.cadstarworld.com

To modify any outline (board, figures, component outlines etc) you can also use the Shape
Properties Window by selecting the outline you can see, and by modifying the absolute or
relative coordinates.

You can also create screw holes or mounting holes if you like. To create any holes within the

board, click the Shape Default icon

and select Cutout. Click any of the drawing tool icons

, click at the board outline and begin drawing a Cutout within the board outline.

If you didn't succeed to draw the board outline or to import the board outline through DXF, just
open

Example1a.pcb

Once the board outline have been imported or draw manually you can set an interactive origin,
displaying X and Y co-ordinates of all design items, and cursor positions, relative to the new

origin. Select Settings

Æ Interactive Origin

and place the origin at the lower left corner of the

board. When you enabled Snap to Endpoint it will be even easier to place the Interactive Origin.

To enable Snap to Endpoint select Settings

Snap

Endpoint

Note: If the Snap toolbar is not visible, goto Tools

Customise

Toolbars and enable Snap.

For the next step, select Actions --> Placement --> Arrange Components

in the menubar,

then select Place Around Board Outline --> Next --> Finish. All components will be placed
around the board outline that you created.

You can now start to place the critical components inside the board outline. In this case, the
pins (for 9V and GND) and the LEDs are the critical components. They should be placed first.

For the next step, select pin VCC9V by clicking on the pin or just type in VCC9V followed by the

return command (it will be highlighted automatically), then click the Item Properties

Icon and

change the

X-position to 250,0 and Y-position to 875,0

Repeat this action for:

Pin AGND, change the

X-position to 450,0 and Y-position to 875,0

omponent LED1, change the

X-position to 250,0 and Y-position to 175,0

and rotate 90°

Component LED2, change the

X-position to 1750,0 and Y-position to 175,0

and rotate 90°

After the placement of all the critical components, you can now place the remaining

components by selecting Actions --> Placement --> Automatic Placement

in the menubar.

You can Enable all Auto Rotation angle in the Automatic Placement window before placing the
components (depending on your design rules). Try the different settings and experience the
different results.

If components do not fit on the board because the board outline is not big enough, you can
always increase the board size.

If you didn't succeed to place the components, just open

Example1b.pcb

You can also move the components manually if you wish, and change to a smaller working Grid

to suit your placement needs (just double-click on the grid button on the bottom

of the window).

Note: you can select any footprint by simply selecting the particular symbol in the schematic. In
CADSTAR, we call it Cross-Probing (No problem with this feature as everything is on the same
GUI). To try it out, select Window --> Tile Vertically in the menu bar first. To continue with the
next exercise, you should activate and enlarge the PCB Design window.

Finally to create a partial power-plane, create a template by selecting the board outline,

choosing Actions --> Duplicate Shape -->

Template in the menu bar and changing the layer

to Bottom Elec.

For more information visit www.cadstarworld.com

Note: Copper pour will be generated automatically in the Embedded Router or P.R.Editor XR
(up to your choice) on solder side based on the template area. Copper shapes will be created
to fill in the empty space within the template outline connected for example to AGND.

After the template has been created, you should set the properties
for this template. To do this, you will first highlight the template

created by you. Then click on Item Property

icon.

You can set the properties as follows:

Name Template: use default name

Relief Copper Code: 10

Layer: Bottom Elec

Signal Name: AGND

Clearance Width: 10

Thermal Relief: Enable On Pads (Angle45°)

Note: Automatic Pour is ENABLED!

[These are the important parameters you need to set]

The steps that were mentioned in this chapter are again a typical sequence. There are other tools
such as Radial Placement, Gate and Pin swap, Replicate Placement etc. to help designers like you to
achieve a correct placement of components.

The completion of placement means you can now start to route the PCB.

Select Tools --> Embedded Router or click the Embedded Router

icon in

the menu bar, to go to the routing environment.

If you didn't succeed to create the template, just open

Example1c.pcb

before going to the routing environment.

Step 3 - PCB Routing for Design A

You are likely to be at the Embedded Router by now, but before
starting any routing we advise you to check the Routing Options.
Setting the Routing Options is very important before any routing!
Select Tools --> Routing Options… in the menu bar or click the
Routing Options

icon.

The "Routing Options" box contains several options for the routing process: Route Width,
Routing Parameters (for autoroute), Routing Angle, On-Line Design Rule Check, Push Aside,
Activ-45 Degree Routing etc. Make sure that at least On-line DRC, Angled Autorouting, Angle
45 Degrees, Activ-45 Degree Routing and Automatic Pour are Enabled. You can use these
options to create the result you want. You can start with manual routing by clicking two icons on

the tool bar, Item Focus

and Manual Route

as shown. Experience the ease-of-use of the

Activ-45 Degree Routing and Automatic Pour starting at the solderside (Bottom Elec), by
selecting a net just once and moving the cursor to the other end of the net.

You can change the active routing layer from Top Elec

to Bottom Elec

(by clicking the Top Elec button on the bottom of the window and changing the Current layer to
Bottom Elec).

While routing, you can insert a Via by using the right-hand mouse button and select Change
Layer.

Or you can change the route width on the fly from Optimal to Necked or Change Width (choose
a width between Min and Max, depending on your Route Assignments).

For more information visit www.cadstarworld.com

You can also use the automatic routing features (usually designers like you will leave this step
to the last, as manual or semi-auto routing is usually necessary for the critical

nets/connections). The two icons used are Net Focus

and Autoroute

and you can auto-

route either net by net or just drag an area around the whole board outline.

Copper pour will be generated automatically on solder side (Bottom Elec), saving you a lot of
time!

Note: the copper poured into the template has followed the properties you have set. The
copper has also automatically avoided the cut-out of the board outline.

After completion, you can go back to the PCB Design Editor window by selecting File --> Exit

Embedded Router in the menu bar or by clicking the Exit Embedded Router

icon. Don't

forget to rebuild the router results into the layout. You can now see a design similar to the PCB
shown below:

At this stage, you can save the file

If you didn't succeed to route the design, just open

Example1d.pcb

to have a look.

This is probably the last stage of the PCB design. It requires some careful considerations as to how the
board can be routed, what are the critical nets, what nets have to be routed manually etc. For
advanced users, more routing features and High-Speed routing are to be considered.

For more information visit www.cadstarworld.com

Step 4 - Manufacturing data for Design A

At this stage, you can also create the manufacturing data (Gerber, N.C.Drill, Parts List, Placement data
etc.) for the manufacturing of the PCB. You can select File --> Manufacturing Export --> Batch

Process… in the menu bar or click the Batch Process

icon. In the Batch Process window you select

Open --> Manufacturing Output 2 Layer.ppf, which you can find in the User directory and click START.

You can easily add more rows to create layers that
you would like to post-process. In this design, since
it is a 2-layer board, the layers that are to be
generated are Top Elec, Bottom Elec, Top Solder
Mask, Bottom Solder Mask, Top Silkscreen (all in
Extended Gerber RS274-X format). Other
additional manufacturing data that can be
generated are Parts List, Placement Data, Drill
Data Plated & Non-Plated (Excellon format), which
is also necessary for manufacturing. All manufacturing data will be saved in the Output directory.

There are other tools such as Associated Dimensioning (Orthogonal, Angular, Radial etc.), Snap,
Component Rename etc. to help designers like you to create all necessary manufacturing data.

Quite interesting?

Check

CADSTAR 3D

, supporting Import/Export of STEPS AP203, AP214, ACIS and STL formats,

providing you an optimized solution for the placement and verification of a PCB Design in its 3D
environment. Replace the board outline, component placements smoothly back annotated and import
other PCB designs and housings, build it all together and run a complete collision check.
It’s not just a viewer!

More information you can find on:

http://www.cadstarworld.com/products_cadstar3d.asp

If you want to continue practicing, go to Design B.

For more information visit www.cadstarworld.com

• Design B

Transistor Audio Amp (50 mW)

formation on Design B - Transistor Audio Amplifier

ere is a little audio amplifier, similar to what you might find in a small transistor radio. The input stage

tep 1 - Schematic for Design B

Design B, you will have to decide what to do based on the knowledge you have gained from your

Study the schematic.

Collect and note information on the components.

From the hand-drawn schematic, you should be able to see eighteen (18) components, they

- 2 x 2N3053 NPN Transistor

- 1 x 470 Ohm Resistor (470E-MRS25-1%)

o (3E3- RS25 %)

EC)

H
is biased so that the supply voltage is divided equally across the two complimentary output transistors,
which are slightly biased in conduction by the diodes between the bases. A 3.3 Ohm resistor is used in
series with the emitters of the output transistors to stabilize the bias current so it doesn't change much
with temperature or with different transistors and diodes. As the bias current increases, the voltage
between the emitter and base decreases, thus reducing the conduction. Input impedance is about 500
Ohm and voltage gain is about 5 with an 8 Ohm speaker attached. The voltage swing on the speaker is
about 2V without distorting and power output is in the 50mW range. A higher supply voltage and the
addition of heat sinks to the output transistors would provide more power. The circuit draws about
30mA from a 9V supply.

In
work on Design A. I will guide you through it to give you some tips. The sequence is the same as
Design A.

a

b

c

are:

- 1 x 2N2905A PNP Transistor

- 1 x 1.5 kOhm Resistor (1K5-MRS25-1%)

- 2 x 1N4148 Diode

- 1 x 5.6 kOhm Resistor (5k6-MRS25-1%)

- 2 x 3.3 Ohm Resist r

-1

- 1 x 47uF/10V Elec. Cap (47uF-10V-EC)

- 1 x 22 Ohm Resistor (22E-MRS25-1%)

- 1 x 1000uF/50V Elec. Cap (1000uF-10V-

- 5 x SOLDEREYE-1MM (for Input, Speaker and 9V supply)

For more information visit www.cadstarworld.com

Create a new schematic sheet (I like Form A1)

Call out components from the library

Place the components on the schematic sheet

Connect the components

Change any net information (remember I like a different Net Route Code for Power & GND)

Save the design

Create the Parts List

Print the design

Transfer the schematic design to PCB (choose '2 layer 1.6mm.pcb' as PCB technology)

you didn't complete the schematic design as described above, just open

Example2.scm

and transfer

tep 2 - PCB Placement for Design B

assume that you completed the schematic design in a breeze. You can now start to place and

Check and/or change the Unit & Grid (25 mill is preferred)

Change Shape Default

If
the schematic to PCB through File --> Transfer to PCB, choose '2 layer 1.6mm.pcb' as PCB
technology.

I
arrange the components on the PCB after the transfer. Again, I will give you some important points to
follow in order to complete the PCB placement.

a

and select Board.

Draw a board outline (size 2000x1500 thou). If you didn't succeed to draw the board outline,

just open

Example2a.pcb

Arrange components around the Board Outline

Manually place the critical components inside the board outline:

0,0

Fix the position of VCC9V, INPUTGND, INPUT, SPK and SPKGND

Place VCC9V at

X-position 150,0 and Y-position to 150,0

Place INPUTGND at

X-position 150,0 and Y-position to 105

Place INPUT at

X-position 150,0 and Y-position to 1350,0

Place SPK at

X-position 1850,0 and Y-position to 1350,0

Place SPKGND at

X-position 1850,0 and Y-position to 105

Cross-probe if it is necessary

Automatically place the other components

. If you didn't succeed to place the components,

Draw one or more templates

just open

Example2b.pcb

(remember Duplicate Shape and do not forget to allocate the

signal name AGND to the template). If you didn't succeed to create the template, just open

Example2c.pcb

, before going to the routing environment.

For more information visit www.cadstarworld.com

Transfer the PCB to Embedded Router

Step 3 - PCB Routing for Design B

ou are now at the final stages of the PCB design. Again, simply follow the steps and you will complete

Manually route any critical nets

Y
your PCB design very soon.

Automatically route all other nets

Exit Embedded Router

If you didn't succeed to complete the design, just open

Example2d.pcb

to have a look.

Design B after Placement & Routing

tep 4 - Manufacturing data for Design B

reate the manufacturing data

WELL DONE! You have now completed the PCB design

heck CADSTAR 3D, supporting Import/Export of STEPS AP203, AP214, ACIS and STL formats,

More information you can find on:

http://www.cadstarworld.com/products_cadstar3d.asp

For more information visit www.cadstarworld.com

• Design C (Place & Route Editor)

esign C I have created for the more advanced users, making use of the P.R.Editor XR2000. Users,

tep 1 - Schematic for Design C

o keep it simple I have already draw the schematics of Design C for you. Just open

Example3.scm

tep 2 - PCB Placement for Design C

Before transferring to P.R.Editor XR2000 you can create a very rough placement manually.

ome connections between U1 and U2 are crossing! To solve select Actions

Gate and Pin

D
who are making regular use of CADSTAR, do prefer more powerful features as available with the
P.R.Editor XR2000, delivering placement and routing functionality within one environment. By the way
all exercises as done for Design A and Design B in the Embedded Router, can be done as well in the
P.R.Editor XR2000!

T
and transfer the schematic to PCB through File

Transfer to PCB, choose ‘Eurocard-160x100.pcb’ as

PCB technology. If you didn't succeed to transfer the schematics design, just open

Example3a.pcb

before going to Step 2.

Place all IC’s with pin 1 to the north, place U1 at the left, U2 in the middle and U3 on the right of
the board. SMD components can be easily placed on both layers, select capacitor C1 (you
have many options to do so), move C1 to the preferred place, click the right mouse button and
select ‘Mirror’ from the pull down menu. Place all capacitors at the solder side of the board.
Note: The color of the components swapped to the other side of the board do change! If you
didn't succeed to place the components, just open

Example3b.pcb

before moving on.

Swap

Automatic Gate and Pin Swap

Start

. When saving the design a back annotation

file *.RIN will be created automatically, contain g all the Gate and Pins swap information,
which can be back annotated to the schematics design. If you didn't succeed to Gate and Pin
Swap, just open

Example3c.pcb

before going on.

Open the schematics design

Example3.scm

and select File

Back Annotation

and select

. Open

Example3c.pcb

and go to the P.R.Editor XR by selecting Tools

P.R.Editor XR

the *.RIN from the Self Teach directory. After saving the design you should de te the back
annotation file.

When transferring to the P.R.Editor a RIF

Export Option window will be showed
automatically. Ensure that

Write Jumpers

from Library

disabled

For more information visit www.cadstarworld.com

Step 3 - PCB Routing for Design C

You are likely to be at the P.R.Editor XR by now, but before

P.R.Editor XR can not only be used for routing your design

Setting the Placement is very

Select a component and move

starting any routing or further placement we advise you to check
the Routing Tool Options (CTRL-T). Setting the Routing Options
is very important before any routing! Select Configure

Routing

Routing Tool in the menu bar. Ensure the settings are equal

to the example. If you don’t like copper to be poured
automatically disable it. If you don’t like routes to be pushed you
can disable Push aside or reduce the Effort in which case less
routes will be pushed aside.

but as well changing your placement without the need to go
back to the Design Editor, but before starting any placement we
advise you to check the Interactive Move and Push Aside
Options. Setting the Interactive Move options by selecting
Configure

Interactive Move in the menu bar is needed to

control component placement.

important before any placement.
Select Configure

Placement

Push Aside in the menu bar. Ensure
the settings are equal to the example.

it. Notice that other components are pushed aside, and when

enough space the selected component jumps over other components. Components can also be

swapped

to the other side of the board or rotated

As the board is a 4 layer board with 2 power planes GND & VCC, we will first start with Stub

routing for the GND & VCC. Select Whole Net Mode

, Auto route

and select the GND

signal (repeat the same for VCC).
Note: By using the customizable Function Keys F5 or F6 you can scroll through the layers from

The next step is to create a footprint. A footprint is a route template that can be applied to an

top to bottom or the other way around.

SMD component. It enables routes to `breakout' from a surface mounted pad using a pattern
that is efficient on space and gets the route to an inner layer as soon as possible. Footprints are
often used and can be easily re-used for BGA’s, QFP’s or even SO-IC’s.

Note: If the footprint toolbar is not visible go to View

Toolbars

Footprint

For more information visit www.cadstarworld.com

Before creating the footprint, goto Configure

Routing

elect Routing

Footprint

Auto

Footprints in the menu bar. Ensure the settings are equal to the
example.

in the menu bar and drag

y using Y-Mirror Footprint

an area around the component U2 or just a number of pads.

or any of the other Footprint

options (like Rotate Footprint) you can modify the footprint as you
like. Once you are happy with the footprint you can save it,

selecting Routing

Footprint

Save

and drag an area

around the created footprint, so you can re-use it within other
designs. Save the footprint as ‘so20-l.fpt’.

Zoom-in on component U3 and select Routing

Footprint

Create Exit Directions

in the

or the next exercise you should open

Example3d.pcb

in the Design Editor and go to the

menu bar and drag an area around the component U3. A window ‘Input Footprint File’ ops up
and you can select the ‘so20-l.ftp’ which you save earlier. You have re-used a footprint
successfully.

F

P.R.Editor XR by selecting Tools

P.R.Editor XR

The P.R.Editor XR will help you to complete your design step by step by using advanced auto-

What is Trunk Routing?

Trunk Routing introduces the concept of the intelligent Trunk object, allowing you to route any

route technologies.

Trunk Routing

will help you to complete data and address lines easier.

given set of signals in an intuitive manner and with as little effort as possible.

For more information visit www.cadstarworld.com

Selecting which connections are Trunk Routed

Busses of data and address lines can be

Í
already designated in a schematics design (as
done in Example3.scm) and transferred to PCB
and P.R.Editor XR. A bus (trunk) can be
selected by the bus marker, zoom in on the bus

marker before selecting Manual Route

Alternative you can double click on one of the

pads as marked by the bus marker, before selecting

Manual Route

. Note: All pads as marked will be

selected and highlighted.

When no bus marker is visible you can drag

Í
a multiple selection around a set of pins before

selecting Manual Route

to start Trunk

Routing.

efore starting any trunk routing we advise you

B
to check the Trunking Options. Select Configure

Routing

Trunking in the menu bar.

For more information visit www.cadstarworld.com

Simple manual routing of a Trunk on a single layer

order to aid routing, snap axes and trunk end routing areas will be drawn on the canvas

o start routing the Trunk you can place the Gather Point by clicking the left mouse button in

be added during Trunk Routing. This can

hen you have added in the required Trunk path, it is possible to finish Trunk Routing in

ey can be used in order to finish Trunk routing at the last added corner position

Trunking Options

dialog,

is also possible to restart the Trunk Router on a previously added Trunk. This can be easily

In
around each of the target sets of pins for the Trunk. You will see

Twist Arrows

drawn on the

canvas showing the best entry angle for the Trunk to the target pins in order to minimize
connections crossed at each end. You will also notice that you have a Gather Point for the
Trunk that is now dynamic on the end of your cursor. The Gather Point defines the start for the
Trunk where all of the parallel tracks will be considered as a single object.

T
the position that you want to start routing the Trunk from. Trunk segments are now introduced
towards the cursor position as you move the mouse on the canvas. Use the left mouse button
to confirm Trunk segments that you have added. A corner can be added by changing direction
of movement of the cursor after a left mouse click.
Note: There are different styles of corners that can
be changed by using the Right Mouse Context Sensitive menu.

W
several ways:
The

'Escape'

or using the Right Mouse Context Sensitive menu

Cancel

option.

With the

‘Single Click Finish on Snap Line’

option selected on t

a single click when positioned over a snap axis will also finish the Trunk. Remember Select
Configure

Routing

Trunking in the menu bar.

done by selecting the manual routing icon

and then picking the Trunk on the canvas, or

selecting the manual routing icon

with the Trunk item already selected

Note: Try also the ‘

Backspace’

key (Remove Previous Item).

During routing of a Trunk the Trunk contents will dynamically reorder to maintain the least

dding Vias while Trunk Routing

o place a Trunk Via pattern while using the Trunk Router, you can double click the left mouse button or

anual Reordering of Trunks and Via patterns

is possible to reorder the contents of a Trunk manually, by manual selection of a single track

anual Trunk End Routing

ou can use the Manual and Activ-45 routers to interactively route the connections up to the

number of crossed connections at each of its ends. This is done to give the best routing pattern
for each end. This option can be configured using the

Trunking Options

dialog

Minimise

Crossed Connection

setting.

T
choose a different layer using the Layer option on the Right Mouse Context Sensitive menu. It is also
possible to change the

Trunk Via pattern style

to a number of predefined styles using the

Right Mouse

Context Sensitive

menu during Trunk Routing or by pressing the

'Tab'

key in order to cycle through the

predefined Trunk Via patterns.

It
inside the trunk using selection preview. Hold down the

‘Shift’

key and press the Left mouse

button. It is possible to switch to one of the other items by pressing the

'Tab'

key. Each time the

'Tab'

key is pressed the next item will be highlighted. You can then drag this track interactively

to another position inside the Trunk.

Y
end of the trunk. During the routing process you can still re-order the trunk if necessary.

For more information visit www.cadstarworld.com

Automatic Trunk End Routing

While you are Trunk Routing, it is possible
to automatically route the ends of a Trunk
using the Trunk End Router. Routing will
be attempted for all Trunk Ends that are
inside a Trunk End Routing target area.
Select Configure

Routing

Trunking in

the menu bar and ensure the settings are
equal to the example.

In some circumstances you may wish to
decompose Trunk objects that you have
added to your design into normal Track.
For example, you may wish to split a
segment of a Bus into Track so that you
can route the Bus around another obstacle.
In order to do this you first need to select
the Trunk items that you wish to
decompose and then use the Decompose
option on the Right Mouse Context
Sensitive menu. Once a Trunk has been
decomposed into Track, it is not always
possible to compose these items back into
Trunks.

You can use the Trunk Routing, Manual and Activ-45 routers to interactively route the
connections up to the end and finish the board.

If you didn't succeed exit the P.R.Editor XR without saving and you will automatically return to
the Design Editor and open

Example3e.pcb

For more information visit www.cadstarworld.com

Auto Routing

For the next exercise you should open

Example3f.pcb

the Design Editor and go to the P.R.Editor XR by

selecting Tools

P.R.Editor XR

Before starting any auto routing we advise you to

change the Routing Tool Options (CTRL-T) again.
Setting the Routing Options correctly is very important
before any routing! Select Configure

Routing

Routing Tool in the menu bar. Ensure the settings are
the same as in the example.

Note: Although Errors are allowed, you should first allow
the router to make some errors. In combination with
Effort 10 the router will continue routing till no errors are
left.

Select Routing

Autoroute

from the menu bar and

drag an area around the whole board outline or part of
the board you would like to auto route. The auto router
will stop automatically once all connections have been
routed. But the routing is not yet optimal, and therefore
you should run first a Smoothing pass. Before running a
Smooth pass select Configure

Routing

Tool in the menu bar and enable Smooth.

Select again Routing

Autoroute

from the menu bar

and drag an area around the whole board outline or part
of the board you would like to smooth.
Note: As a result of the smoothing pass the number of
vias and segments will reduce.

If you didn't succeed exit the P.R.Editor XR without
saving and you will automatically return to the Design
Editor and open

Example3g.pcb

which I finished for you

manual, before going to the next step.

For test reasons you can decide to automatically

generate a testpoint on every node (or as many as
possible). Before starting any allocation of testpoints,
select Configure

Routing

Testpoints and make

sure the settings are equal to the example. Do not forget
to select ‘(Bottom Elec)’ in the section Layers!

Select

Select

All from the menu bar and note that all

will be highlighted. Select Routing

Testpoint

Allocate

and the testpoints will be added

automatically. Select Utilities

Reports

Testpoints to

create a testpoint report as in the example.

Note: Now that you have finished the design, you can
select File

Exit from the menu bar.

If you didn't succeed to finish the testpoint creation, just
open

Example3h.pcb

For more information visit www.cadstarworld.com

•

Design D (Single Sided Board Design)

Transistor Audio Amp (50 mW)

esign D is based on the same schematics as Design B (a little audio amplifier). But this time you will

Step 1 - Design D

. Open

Example2.scm and transfer the schematic to PCB through File --> Transfer to PCB…, but

tep 2 - PCB Placement for Design D

ou can now start to place and arrange the components on the PCB after the transfer. Again, I will give

Check and/or change the Unit & Grid (25 mill is preferred)

Change Shape Default

Information on Design D - Transistor Audio Amplifier

D
create a single sided board and I will show you how to add jumpers on the fly. Typically, a jumper is
used to bridge across other routes, the jumpers discussed here are non-functional jumpers and do not
appear in the schematics. I will guide you through it to give you some tips. The sequence is the same
as before.

now choose '

1 layer 1.6mm.pcb

' as PCB technology instead. This default technology file I

prepared already for you and you will notice although I’m using the same library that the solder-
pads are larger, thicker track-widths and more spacing have been defined.

Y
you some important points to follow in order to complete the PCB placement or you can go
immediately to

Step 2.i

. When creating a single board design a good placement is highly important to

avoid crosses in the connections, so take your time. If you don’t succeed 100%, don’t worry as you will
be able in Preditor to add jumpers on the fly, just like adding a via

a

and select Board.

Draw a board outline (size 2000x1500 thou). If you didn't succeed to draw the board outline,

just open Example4a.pcb

Arrange components around the Board Outline

For more information visit www.cadstarworld.com

Manually place the critical components inside the board outline:

0,0

Fix the position of VCC9V, INPUTGND, INPUT, SPK and SPKGND

Place VCC9V at

X-position 150,0 and Y-position to 150,0

Place INPUTGND at

X-position 150,0 and Y-position to 105

Place INPUT at

X-position 150,0 and Y-position to 1350,0

Place SPK at

X-position 1850,0 and Y-position to 1350,0

Place SPKGND at

X-position 1850,0 and Y-position to 105

Cross-probe if it is necessary

Automatically place the other components

. If you didn't succeed to place the components,

Before going to the routing environment check out Libraries

PCB Components

just open Example4b.pcb

. Open

Example4b.pcb and go to the P.R.Editor XR2000 by selecting Tools

PReditor XR…

Jumpers. I have created already some pre-defined jumpers, which you will be able to select in
Preditor on the fly.

For more information visit www.cadstarworld.com

Step 3 - PCB Routing for Design D

ou are now at the final stages of the PCB design. Simply follow the steps and you will complete your

You are likely to be at the PReditor XR… by now, but before

Tip: By using the customizable Function Keys F5 or F6 you can

Y
PCB design very soon. When transferring to the Preditor a RIF Export Option window will be showed
automatically. Ensure that

Write Jumpers from Library

is this time

enabled

starting any routing we advise you to check the Routing Tool
Options. Setting the Routing Options is very important before any
routing! Select Configure

Routing

Routing Tool… in the

menu bar (or use CTRL-T). Ensure the settings are equal to the
example. If you don’t like copper to be poured automatically
disable it. If you don’t like routes to be pushed you can disable
Push Aside or reduce the Effort in which case less routes will be
pushed aside.

scroll through the layers from top to bottom or the other way
around. Select in the menubar Layer, change the Current Layer
to Bottom Elec and select OK.

Note: 2 layers have been added (Top Jumper and Bottom Jumper)!

For more information visit www.cadstarworld.com

b. Manually

route

the net between resistor R2 and capacitor C2 as in the example

ide

In the next step you will add a jumper on the fly by manually routing

below on the solders

the net between transistor TR1 and resistor R2 as in the

low on the solderside. Route to the location you want to

add the first pad of the jumper and double click, select Top Jumper.
Now move the cursor to the location you want to add the second pad
of the jumper. Preditor will show you a thin line representing the pitch
of the pre-defined jumpers depending on the available space. Double
click again will add the jumper and you can continue routing. Preditor
will show you only a list of pre-defined jumpers if more then one
jumpers with the same pitch have been defined in the library. It’s

example be

as ea

Now route all the connection on solder side and insert jumpers if necessarily till no connection

sy as adding a Via!

are left.

For more information visit www.cadstarworld.com

Once you have finished the design you can select File

Exit from the menubar

All routing and jumpers will be nicely back annotated to the PCB Design. Running ECO update

If you didn't succeed to complete the design, just open Example4d.pcb to have a look.

Design D after Placement & Routing

Step 4 - Manufacturing data for Design D

t this stage, you can also create the manufacturing data (Gerber, N.C.Drill, Parts List, Placement data

d

e

won’t remove jumpers and the jumpers will appear normally in the Part list and Placement data.

A
etc.) for the manufacturing of the PCB (as you did also for Design A). You can select File -->

Manufacturing Export --> Batch Process… in the menu bar or click the Batch Process Icon

. In the

ou can easily disable the rows that you would not

Drill

ich

lternative you might want to produce an ODB++ output file. ODB++ is one of the most intelligent

Batch Process window you select Open --> Manufacturing Output 2 Layer.ppf, which you can find in
the User directory and click START.

Y
like to post-process. In this design, since it is a
single layer board, the layers that are to be
generated are Bottom Elec, Top Solder Mas
Bottom Solder Mask, Top Silkscreen (all in
Extended Gerber RS274-X format). Other
additional manufacturing data that can be
generated are Parts List, Placement Data,
Data Plated & Non-Plated (Excellon format), wh
is also necessary for manufacturing. All manufacturi

g data will be saved in the Output directory.

A
CAD/CAM data exchange format available today, capturing all CAD/EDA, assembly and PCB
fabrication knowledge in one single, unified database. The output produced by this option can b
viewed graphically on the viewer provided by Valor.

WELL DONE! You have now completed the PCB design

For more information visit www.cadstarworld.com

Podsumowanie

Po tych czterech ćwiczeniach powinieneś znać podstawowe zasady projektowania płytek drukowanych.
W niedalekiej przyszłości być może będziesz projektować bardziej skomplikowane projekty PCB
używając jednego z najbardziej zaawansowanych systemów EDA jakim jest CADSTAR.

Wraz z tą broszurą otrzymałeś darmową wersję CADSTAR Express, która ograniczona jest do 300 pinów
i 50 komponentów.
CADSTAR Express możesz również ściągnąć z naszej strony

www.cadstar.pl

Aby otrzymać pełną 30-dniową wersję ewaluacyjną CADSTAR prosimy o kontakt na emaila

sales@quantumeds.co.uk

. Jest ona darmowa i uzyskać ją można podając swoje dane oraz adres

fizyczny komputera (physical address)

Adres fizyczny można znaleźć w następujęcy sposób:
Start/run [wpisz polecenie] cmd [enter]
[wpisz polecenie] ipconfig /all [enter]

Istnieją również inne narzędzia CADSTAR, które pomagają konstruktorom w projektowaniu elektroniki.

CADSTAR P.R.Editor XR2000/5000 S or HS - High-Speed Circuit Design Routing (trunking, stub,
memory, track length, delay, differential pair, impedance controlled routing) & Placement
CADSTAR P.R.Editor Rules by Area - Different technology-rules to different areas of the PCB
CADSTAR EMC Adviser - EMC rule check on PCB layouts
CADSTAR SI Verify - Post Simulation for reflection, cross-talk
CADSTAR Variant Manager - One Schematics & PCB - many different requirements
CADSTAR Design Viewer - To view all CADSTAR designs (free to download)
CADSTAR 3D - 3D Verification, back annotation of changes, supporting STEP, ACIS & STL
CADSTAR Exchange Library - Over 220.000 CADSTAR parts available for download from LinkZ (only
available in combination with a valid maintenance agreement)
CADSTAR Datasheet Publisher - Extracts parts information from library in HTML datasheet
CADSTAR IDF Advanced 3D interfaces - between MCAD and PCB design systems
CADSTAR SPICE A/D simulator interfaces – TopSPICE, PSpice & B2 SPICE
CADSTAR MRPLINK - Synchronization, parts management, history management and BOM
management
CADSTAR Thermal Analysis Interface
CADSTAR Microstrip Routing Option for RF Design
CADSTAR Docsymbol Generator (Import BMP, GIF, JPG, PNG)
CADSTAR Schematic Symbol Rename
CADSTAR Signal Reference Annotation
CADSTAR Assembly Name Generator
CADSTAR Drill Table Generator
CADSTAR Gerber reader
CADSTAR GENCAD Output
CADSTAR Panelizing, Editing
CADSTAR Migration from P-cad, Protel or Orcad - Schematics, PCB design & Library

Więcej informacji na stronie

Document Outline