Layer Table and Defining Layers - LAB

Use the Tables pull down menu or the “y” hotkey to access the Layer Table. 


Refer to the layer definitions in the Readme text file in the Gerber file directory for the correct layer Types.


Assign Draw and Flash colors. Then exit the menu.




Experiment

• Can you figure out what the file types are by looking at the layers?

• What happens to the colors in the Layer Bar?

• Can you change the layer names?

• Turn off all but two layers. Set one of the layers to Ref using the status button. 

           What happens when you redraw the display? 

• What happens if you try to select an object on the REF layer? 

           (Use Edit/Move or Copy as a selection device).

Layer Table and Defining Layers - Video

Here is a demonstration of the Layer Table setup procedure:

Layer Table and Defining Layers

Use the Tables pull down menu or the “y” hotkey to access the Layer Table.

The layer table is used to set the layer Type, and assign Draw and Flash colors. 
It can also be used to set the Active layer (the layer that remains on when all others are turned off) and the Top layer (the layer that redraws last and therefore appears “on top” in the screen display). 


The Data column indicates whether or not the layer contains any data.


(Note that the layer numbers correspond to the numbers in the layer bar.)

Layer types are selected from a pull down menu that is accessed from a cell in Type

column of the layer’s row.

Select the appropriate layer definition from the available options.

Note: 

Whether a plane is positive or negative has nothing to do with its electrical characteristics

but with whether the photo file represents a positive or negative image. “Positive Plane”

layers are processed the same as “Internal” layers

Colors are selected from a chart that pops up by clicking the Draw or Flash cells. 

Color selection is purely a matter of user choice. Try to select familiar draw colors that will help you recognize layers on sight. Choose a different (preferably dark) color for flashes.

In addition to the ability to turn layers On and Off the Layer Table can set a layer to “Ref”

(for reference). In this condition objects on a layer can be viewed but can not be selected.

A video demonstrating Layer Table and Defining Layers will be posted on the next blog post.

Ordering Layers - LAB

From the Edit pull down menu, select Layers/Reorder.

(Note the layer order as it appears in the Active Layer pulldown window.)

On the Reorder Layers popup menu, click on a line item and drag it to a new location in the layer order.

When all layers have been placed in the desired order, click on the Renumber button.

Exit by clicking on the OK button with the LMB.

(Note the layer order as it now appears in the Active Layer pulldown
window.)

Ordering Layers - Video

Here's how ordering layers is done in CAM350:

Ordering Layers

Each Gerber file that has been imported represents a “Layer” of the design. 


If we could see a cross section of the design we would see that each of these layers occupies a unique physical space from top to bottom. Putting the layers in a specific order is more of a user choice issue than an operational requirement. In fact, the order means nothing. It’s simply conducive to the sanity of the user.


From the Edit pull down menu, select Layers/Reorder.

When the Reorder Layers popup menu appears, 

click on a line item and drag it to a new location in the layer order.

Before Reorder

After Reorder

When all layers have been placed in the desired order, click on the Renumber button.

This will assign a new layer number that corresponds to the numbers on the layer bar.

Exit this menu by clicking on the OK button with the LMB.

The next blog will show a demonstration of the Layer Reordering procedure.

Importing Gerber and Drill Data - LAB

Use File/New to begin a new CAM350 session.

Select File/Import/Auto Import and set a path to the PCB2CAM350/

Gerber directory.

Set the button for Metric, then select Finish. 

Cam350 will automatically select and load the Gerber and NC drill files.

During the loading process a message will pop up warning of “Unassigned Tools. 

This concerns drill sizes which have not yet been set and is normalbehavior.

Note: Because this demonstration board has Blind and Buried vias the

             message pops up 3 times. Once for each drill set.

Experiments:

• What happens when you load the files with set the button set to English?

• What happens when you select Next instead of Finish?

Make sure the Gerber and Drill files are loaded correctly before proceeding.

Use the Settings/Units pull down menu and select Metric.

Use the File/Save As command at this point to open a new CAM350 database for this design. Set the path to your practice area and assign the file a unique name (i.e. don’t use the same name as the Demo files).

Use the CAM_Demo_Offset.CAM file as a reference if you have any questions.

Note: the dot “CAM” file extension denotes a native CAM350 formatted file.

            CAM350 files are Opened using File/Open.

Importing Gerber and Drill Data - Video

Here's how to import gerber and drill data using CAM350:

Importing Gerber and Drill Data

Use File/New to begin a new CAM350 session.

Then, select File/Import/Auto Import. 

Set a path to the directory that contains the Gerber and NC Drill data. 

Select the appropriate button for English or Metric, then select Finish. 

Cam350 will automatically select and load the Gerber and NC drill files 

(selecting Next allows the user to select the files that will be loaded).

If you’re a PowerPCB user you will see a pop up warning of “Unassigned Tools.

This concerns drill sizes which have not yet been set and is normal behavior.

A video tutorial to show this process will be posted on the next blog.

Subscribe to this blog and learn more about using CAM350 for PCB Designers.

Creating an IPC-D-356 Netlist - LAB

The utility CAM350 uses to produce the IPC-D-356 netlist is an installation option. 


If you haven’t purchased the CAM350 CAD to IPC option you will not be able to perform this step. Instead, use the CAM_Demo_IPC.Net file provided in the Lab demonstration materials. 


Open a new session of CAM350. 


Using File/ Import > CAD Data select the PowerPCB CAD format. 


Set a path to Cam_Demo.ASC and Open it. 
(It’s not necessary to Extract Polygons for net checking and you can acknowledge the warnings that follow). 


Once the ASCII file has loaded, Export the IPC-D-356 netlist using the File/Export > Netlist > IPC-D-356 option. 


Set a path to your practice directory, assign a filename for the netlist and Save it. 


There is no need to save the imported ASCII file once the IPC-D-356 netlist has been saved.

Creating an IPC-D-356 Netlist - Video Tutotial

Here's a video on how to create an IPC-D-356 Netlist in CAM350:

Creating an IPC-D-356 Netlist

Verification of photo plots to the original design database is made possible by an IPC-D-356 Netlist. This type of netlist consists of connection information in an ordinate format – or a virtual 3 dimensional description of any net. 

Take a look at the following examples of netlist formats:

A simple netlist, such as might be generated by typical schematic capture software consists only of part/pin connection references.

Schematic Netlist:

*SIGNAL* NET_1
U1.1 U2.1


The same IPC-D-356 netlist connection generated from the CAD database by CAM350 would look like this:

CAD Data IPC Netlist:

317NET_1 VIA MD 500PA00X+ 2700Y+ 2000X1000Y S0
317NET_1 VIA MD 500PA00X+ 13400Y+ 2000X1000Y S0
327NET_1 U1 -1 A01X+ 2690Y+ 4550X 600Y2100 S2
327NET_1 U2 -1 A01X+ 13390Y+ 4550X 600Y2100 S2


And the same extracted net from the fabrication data by CAM350 would look like this:

Extracted Netlist:

317$Net0 VIA MD 500PA00X+ 2700Y+ 2000X1000Y S0
317$Net0 VIA MD 500PA00X+ 13400Y+ 2000X1000Y S0
327$Net0 VIA A01X+ 13390Y+ 4550X 600Y2100 S2
327$Net0 VIA A01X+ 13400Y+ 3000X 150Y S2
327$Net0 VIA A01X+ 2690Y+ 4550X 600Y2100 S2
327$Net0 VIA A01X+ 2700Y+ 3000X 150Y S2


Whether you can read this or not doesn’t matter, that’s what the software’s for.


CAM350 uses the PCB design database (as opposed to Gerber and NC drill data) to produce the reference IPC-D-356 netlist to which the fabrication materials will be compared.

Begin by opening a new session of CAM350.

From the File pull down menu, import CAD Data and select the appropriate CAD format.

Set a path to the ASCII file and Open it.

Numerous queries and warnings will pop up. For the purpose of creating the IPC-D-356 netlist, it’s not necessary to Extract Polygons for net checking.

…and you can acknowledge the warnings that follow.

Once the ASCII file has loaded, Export the IPC-D-356 netlist:

From the File/Export/Netlist select the IPC-D-356 option.

Click OK with the LMB, set a path and filename for the netlist and Save it.

There is no need to save the imported ASCII file once the IPC-D-356 netlist has been saved.

CAM350 User Interface LAB

Open CAM350 using the icon on your desktop
or Start > Programs > CAM350 V7.5.

Lab sections will often direct your attention to areas in CAM350 window so the following is a review of the User interface and the names that will be referred to.

The Status Bar consists of the following components:

• The left section (0,0:0,0) is readout of the cursor X-Y position in project units.

• The center area (Select Command) shows the status of any command that may be active.

• The right area consists of 5 “buttons” which toggle their functions as follows:

                      “Z” causes the cursor to snap to an object. In this mode the cursor will snap to 

                             the center of a “Flash” or the end of a “Draw”.

                      “S” enables the cursor to snap to the grid (as set by the Snap pull down selector

                             from the Toolbar pull down).

                     “V” toggles the grid display on and off.

The Panorama Bar shows a “Thumbnail” picture of the viewing area referenced to the design extents in a “Window Pane” that may be moved around in the work area.

CAM350 User Interface

The CAM350 Window consists of a:

• Menu Bar
• Tool Bar
• Layer Bar
• Working Area
• Status Bar 
• and “Panorama” window pane.

The Toolbar, Layer Bar, Status Bar and Panorama Windows are enabled from the View Pull down menu.

Other viewing functions include: Window, (Zoom) All, Redraw, (Zoom) In and Out, and Pan

functions may also be accessed from the View menu. (Pan isn’t a pan in the true sense – it re-centers the view at the current cursor location).

Note that to the right of each of these keys is a “hotkey” that may alternately be used to perform the function.

The other pull-down menu options will be discussed in order of relevance as we progress through this tutorial.

The appearance of the Toolbar will vary according to the function being performed but there are always three pull down selections available.

From left to right they are:

1. The Grid setting. 

    This pull down options lets the user select the Grid-Snap spacing.

2. The second pull down is the Active D-Code selector. 

     It has no practical application in this context.

3. The Active Layer pull down selection sets the “Active Layer”. 

    The active layer is noted by a red box in the cell (No. 1) and indicates the layer that will 

    not be turned off by an All Off command. A blue box (No.16) indicates the layer that 

    appears “on top” of the display.

Note that the pull down selector has the full name of the photo plot or NC

Drill file associated with a particular layer number.

The Status Bar has 3 parts:

1. The left section (0,0:0,0) is readout of the cursor X-Y position in project units.

2. The center area (Select Command) shows the status of any command that may be active.

3. The right area consists of 5 “buttons”…>

which toggle their functions as follows:

“Z” causes the cursor to snap to an object. In this mode the cursor will snap to the center of a “Flash” or the end of a “Draw”.

“S” enables the cursor to snap to the grid (as set by the Snap pull down selector from the Toolbar pull down).

“V” toggles the grid display on and off.

The “T” and “H” have no relevance to this tutorial.

The status of these buttons can be changed either by pressing the corresponding keyboard key or by placing the cursor over the button and “clicking” the Left Mouse Button (LMB).



The Panorama Bar shows a “Thumbnail” picture of the viewing area referenced to the design extents in a “Window Pane” that may be moved around in the work area.

CAM350 LAB for PCB Designers

All the materials you need to perform the same operations as in the companion tutorial are provided to allow you try out the features that have been demonstrated (provided you  have CAM350). 


They consist of: 

• PowerPCB files: A PCB file of the demo board (not used but are provided for reference). 

• An ASCII file (can be used to create an IPC-D-356 netlist). 

• An IPC-D-356 netlistGerber and NC Drill files 

• CAM350 files: Some of these files will be used to try out certain features of CAM350. Others, as a reference for comparing your results. 

It is suggested that you create a new directory on your local drive where these materials can be copied from the CD.

CAM350 for PCB Designers - Overview

CAM350 is a multi-use tool for printed circuit board design and fabrication. It can be used to verify CAM materials that have been created by other PCB design tools such as PowerPCB or Cadence. It can be used to prepare those same materials for various processes such as step and repeat, panelization or adjusting feature sizes to compensate for fabrication variables. It can even be used to design a PCB board from the ground up or reverse engineer a PCB design from existing photo plots.


This tutorial will focus on the first of these applications – using CAM350 to verify Gerber and NC Drill data that has been created by another PCB design tool.


Now, all PCB design tools have DRC (design rule check) utilities to verify connectivity and spacing rules. But these utilities only check the rules against the Design Database. CAM350 has the ability to check the design database against the actual materials that will be used to manufacture the PCB. This adds an extra layer of protection from errors that can be
introduced either inadvertently by incorrect settings in the utility used to generate the fabrication materials, or the potential inability of the design software to detect certain errors.


Additionally, we’ll look at the output capabilities of CAM350 to create check plots, Gerber and NC files, and a “smart” ODB++** database that is compatible with Valor-Genesis software.


The necessary steps will typically be explained with text and graphics. However, most operations will also be demonstrated with “live action” using on-screen digital video media.


You do not need any special software installed to use this tutorial.


Materials for this tutorial were created using PowerPCB V5.0.1 and CAM350 V7.5.2.


* CAM350 is a registered trademark of Downstream Technologies
** ODB++ is the property of Valor Computerized Systems
# PowerPCB is a registered trademark of Mentor Graphics