MULTI CHANNEL DESIGN WITH A FLAT PROJECT
Multi-channel PCB designs have identical or nearly-identical circuitry reproduced for each channel. Replicating circuitry on a PCB design is a simple process in Altium Designer when true hierarchical schematics are employed. However, flat design oﬀers unique challenges that make PCB circuit replication a bit more complex. This paper will instruct the user on overcoming these challenges. At the end of the paper, you will find handy checklists to aid you with using the concepts presented.
TOPICS IN THIS SOLUTION
Altium Designer oﬀers many methods for multi-channel PCB design (i.e. repeating circuitry within a single design). For example, users can set up a project as a hierarchical design and utilize sheet symbols to replicate the circuits within the design. Multiple sheet symbols can reference the same underlying schematic document, or a single sheet symbol can use the Repeat keyword to instantiate the circuit as many times as needed. The main advantage here is that any change to the underlying circuit need only be made once and that change will immediately be seen in every instance. This is a very powerful and eﬃcient method of working with multi-channel designs for a flat project.
Working with these repeated circuits within the PCB document is also extremely eﬃcient. Altium Designer will automatically create a “room” for each iteration of the circuit. Then, you only need to place and route just one of the circuits. Using the Copy Room Formats feature, the placement and routing data can be automatically copied to each subsequent circuit. This makes the layout of repeated circuits extremely simple, no matter how many there are!
There are many users, however, who have not worked with hierarchical designs and feel more comfortable using a flat design methodology. Or, some projects may just be too simple to warrant setting the entire design as hierarchical. Whatever the case, there are a number of legitimate occasions wherein the project is set up as flat, but circuit replication is necessary and the layout of that circuit also needs to be replicated.
There are two scenarios that need to be addressed. Each has its own steps to set up the PCB document accurately, to enable reuse of the placement and routing data. The first possibility is that each repeated circuit is large enough to take up most, if not all, of a schematic capture sheet. Thus, a circuit repeated three times would require three schematic documents—for example, if a system has a large power supply that requires triple redundancy. A second possibility is that the repeated circuit is small – perhaps just three or four components – but it is used many, many times, such as in a small LED circuit. In this case, creating separate sheets for each circuit is obviously not very eﬃcient. It may be more reasonable to have that circuit repeated multiple times as part of just one schematic document. Each of these methods translates to the PCB in a surprisingly diﬀerent way. Both methods are covered here.
By far the easier of the two methods is the use of a separate sheet for each circuit. This is because Altium Designer will automate more of the process in this case. In fact, there will be only one bit of manual intervention required by the user in the PCB document during the process. In the following example, the circuit below is to be replicated just once, creating a Channel1 and Channel2:
Example - Circuit is replicated, creating Channel 1 and Channel 2
PCB Schematic Design Creation
Start by creating the initial circuit on the first schematic sheet of a Printed Circuit Board project (named Channel_1.SchDoc in this example). Then add a second, empty schematic sheet (Channel_2.SchDoc) to the project. The Channel_1 circuit now needs to be copied and pasted to Channel_2. If the reference designators have already been set for the base circuit, go to the DXP menu and then to Preferences. Expand the Schematic group and select Graphical Editing as illustrated in Figure 1. In the Options area, enable the Reset Parts Designators on Paste option.
Figure 1: Resetting the reference designators.
Group-select the base circuit, copy it, and paste it to Channel_2 (Figure 2). Make any edits necessary to the second circuit to ensure proper connectivity with the rest of the design. In this case, the “Pulse1” and “Peak1” ports have been made unique, as has the “Channel 1” text identifier .
Figure 2: The circuit from Channel 1 has been pasted to create Channel 2.
Add whatever additional sheets are necessary for the design. However, it is important that no further additions or changes be made to any of the repeated schematic sheets. Doing so may cause the Copy Room Formats feature to fail later on. For this project, a third sheet (“Connector.SchDoc”) will be added to include a connector with the design.
Since the reference designators on Channel_2 have all been reset, run Tools/Annotate Schematics Quietly to set the designators (Figure 3).
Figure 3: Reference designators have now been reset.
Another important point has to do with multi-part components. In this example, only three of the four op amps in the TL074ACD are being used (A, B, and C), while op amp D is not. Make sure that when the reference designator annotation is done, unused parts from one circuit are not used in another. There must be consistency between each physical circuit so that the routing can match. Here, U1A, U1B, and U1C are used in Channel 1, but U1D does not get used for Channel 2. Instead, Channel 2 starts oﬀ at U2A.
Circuit Board Project Options Setup
The next step is to set the Project Options to automate the component class and room generation. Go to Project/Project Options and switch to the Class Generation tab.
Ensure that the checkboxes for Component Classes and Generate Rooms are enabled for all multi-channel sheets, as seen in Figure 4. Any other sheets are optional. Close the Project Options dialog and save all schematic documents, as well as the project file.
Figure 4: Check the proper Component Classes and Generate Rooms boxes.
PCB LAYOUT DESIGN
Create and save a new Circuit Board file, then use Design/Import Changes… to populate the board. Ensure that the ECO includes the creation of the Component Classes and Rooms (Figure 5). If not, recheck the Project Options setup done previously.
Figure 5: Create the Component Classes and Rooms.
The PCB will then be populated with the Rooms as shown in Figure 6.
Figure 6: The Printed Circuit Board has been populated with Rooms.
Next, move the Channel_1 Room into the board area, then place and route it as desired. Resize the Room outline if necessary (Figure 7).
Figure 7: You can resize the Room to see more detail.
Note: The following section detailing the creation of a Design Channel Class is optional when the circuit only needs to be repeated a couple of times. The Copy Room Formats command will operate correctly when copying a single Room format to another, as is the case in this example. If the Room’s format needs to be copied to subsequent Rooms, however, the command will have to be issued multiple times. It is, therefore, a best-practice to create the Design Channel Class as detailed here.
The next part of the process is to use the Copy Room Formats feature to replicate the placement and routing. Before that happens, however, you must inform Altium Designer that Channel_1 and Channel_2 are the same circuit type. This is done by creating a Design Channel Class.
When a hierarchical structure is used to replicate circuits, the system inherently knows that the circuits are the same, based on the fact that the sheet symbol references the same circuit multiple times. Since these circuits were merely copied and pasted, the information is not automatically created. It is possible that one of the circuits was modified by the user so that there is no longer a match between them. If this is the case, the replication of layout information may not be possible. Since no modifications were made to either circuit in this case, the replication can proceed.
Go to the Design/Classes menu. Note that there is a Component Class for each channel. These were automatically created via the Project Options setting and are also used to define the contents of each Room. Near the bottom of the Object Classes list is an entry for “Design Channel Classes.” Right-click on that group and select Add Class. This creates an item called “New Class.” Right-click the “New Class” name, select Rename Class, and change the name to “Circuit_1.” This renaming step is optional, but if there is more than one circuit type being replicated, it will make it easier to keep track of them.
The members of a Design Channel Class are called Component Classes. Note that the “Channel_1” and “Channel_2” Component Classes are listed in the Non-Members list. Select them both and click the arrow, to move them to the Members list, shown in Figure 8.
Figure 8: Move Channel_1 and Channel_2 to the Members list.
Then, close the dialog. Set the board’s display so that both Rooms are visible. Go to Design/Rooms/Copy Room Formats. The cursor will now change to a large cross-hair, and the Status Bar will instruct you to choose the Source Room. Click anywhere inside the Channel_1 Room. The Status Bar then instructs you to choose the Destination Room. Click anywhere inside the Channel_2 Room. The Confirm Channel Format Copy dialog will then open and present several copying options, as well as a list of all Rooms in the Design Channel Class that are available to copy to. Ensure that Channel_2 has the Copy checkbox enabled. If not, the Apply to Specified Channels checkbox may need to be enabled to access the Copy checkbox.
In the Options area, ensure that Copy Component Placement, Copy Routed Nets, and Copy Room Size/Shape are enabled. Also ensure that Channel to Channel Component Matching is set to, “Match Components By Channel Oﬀsets.” We’ll discuss Channel Oﬀsets in more detail for the second replication method.
Figure 9: Be sure the Copy boxes are checked.
Clicking OK runs the copy routine. The system will look for matching components and connections and duplicate the placement, routing, and Room shape as best it can.
The Channel_2 Room outline now has an identical shape to the Channel_1 Room, and the placement and routing from Channel_1 has been copied to Channel_2. It can now be moved to your desired location on the board.
The final connections between Rooms, and from the Rooms to the rest of the design can now be completed.
Figure 10: Channel 2 has now been placed on the Printed Circuit Board.
FLAT DESIGN USING A SINGLE SHEET
The second multi-channel situation makes use of a much smaller circuit, copied and pasted many times within the same sheet. In this case, it would not be very eﬃcient to create a separate sheet for each circuit, as in the previous example. As mentioned, though, this method requires a few more manual steps for Copy Room Formats to correctly function.
For this project example, we’ll use a very simple design, consisting of six instantiations of the following circuit plus one connector, shown in Figure 11.
Figure 11: This is the example circuit that will be replicated for six instantiations.
PCB Schematic Creation
Start by creating the base circuit. Leave the reference designators at their default “?” state. Group-select the circuit and use the Edit/ Rubber Stamp function to place five more copies of the circuit (Figure 12).
In the previous example, it was important that other components NOT get added to any of the multi-channel sheets. This has to do with Channel Oﬀset values, which we’ll discuss in just a moment. In this example, however, it IS acceptable to place other components to multi-channel sheets. The complete design here adds a connector. Use Tools/Annotate Schematics Quietly (or any other annotation method) to set the reference designators.
Figure 12: The Edit/Rubber Stamp function reproduces the circuit five times.
Channel Offset Values
Before continuing with the next step, the concept of a channel oﬀset needs to be introduced. The main way the Copy Room Formats function attempts to match components from Room to Room is by checking if two components share the same channel oﬀset. This is an integer value that Altium Designer places on each component as it is passed to the Printed Circuit Board, and it is essentially the component’s relative physical position within the schematic sheet.
In the previous example, the Channel Oﬀset values (accessible in the PCB document, in a component’s Properties) for Q1 and Q2 match (Figure 13).
Figure 13: Note that the Channel Oﬀset values are the same for both transistors (Q1 and Q2).
They match because the circuits on the Channel_1 and Channel_2 sheets are identical, so the positions of Q1 and Q2 are the same on each sheet. Figure 14 shows the Channel Oﬀsets match for each like component in Channel_1 and Channel_2.
Figure 14: The Channel Oﬀset values are shown next to each component in red.
Note how they are identical for Channel 1 and Channel 2.)
Channel Oﬀset values are sequentially applied to all components on a schematic. On the single sheet example, all components will thus get unique Channel Oﬀset values. However, that will not allow Copy Room Formats to match components from circuit to circuit. Therefore, the Channel Oﬀset values will need to be manually adjusted within the Circuit Board file. This is easy to do, but it is important to keep the relative order of the components within the copied circuits as they were and not make any changes to their placement or reference designators. We’ll get more into that later.
Component Class Creation Design Guidelines
With the multi-sheet method, Component Classes for the replicated circuits were created automatically, because of the settings in Project Options. With a single sheet, the automated class would include all of the components on the page. However, the Rooms need to be based on just the individual circuits. Therefore, the Component Classes must be manually created on the schematic sheet.
A user-defined Component Class is created by adding a parameter to each component called “ClassName,” with the value being the name of the class as it will appear in the PCB Design. Of course, editing the properties of each and every component in the schematic would take some time. Altium Designer has a couple of options to add the “ClassName” parameter information to groups of components, and both will be used here for demonstration purposes.
Go to Tools/Parameter Manager. Set the Options dialog to include only the Parameters owned by “Parts.” Click Add Column… to add a new Parameter to every component in the design. Enter “ClassName” In the Name field and enable the Add to all objects checkbox. Leave the Value field blank.
Figure 15: Name the parameter “ClassName” and check Add to all objects.
Click Accept Changes (Create ECO) then click Execute Changes to complete the addition of the parameters. Click Close to dismiss the ECO dialog.
Now each circuit will need to be labeled with a unique ClassName, so they each create their own Component Class in the PCB Design. Group-select the entire first circuit. Open the SCH Inspector panel (View/Workspace Panels/SCH/SCH Inspector or F11). Pin the panel in place. Set the filter at the top of the panel to “Include only Parts from current document”.
Figure 16: Group-select the components in circuit 1.
Scroll to the bottom to locate the Parameters section. Set the value of the “ClassName” parameter to “Ch1” and hit the Enter or Tab key.
Group-select the next circuit on the schematic sheet and set the “ClassName” parameter in the Inspector panel to “Ch2.” Repeat for all of the circuits through “Ch6.”
Note that the “ClassName” parameter and values could have been created entirely using the SCH Inspector panel. However, it required a bit less typing to add “ClassName” once using the Parameter Manager, so that was the method we used here.
Figure 17: In the SCH Inspector dialog, set the filter to “Include only Parts from current document”.
Figure 18: Give the “ClassName” the name “Ch1”.
Before transferring the schematic information over to the Printed Circuit Board, there’s one last step in setting the Class Generation tab in Project Options. In this case, the automatic component class generation should be disabled. However, the “Generate Component Classes” and “Generate Rooms for Component Classes” options still need to be enabled in the User-Defined Classes section: see Figure 19.
Figure 19: The Component Classes box has been unchecked. Leave the “Generate Component Classes” and “Generate Rooms for Component Classes” enabled checked.
PCB Layout Guidelines
Create and save a new PCB schematic file, then use Design/Import Changes… to populate the board. Make sure that the ECO includes the creation of the “Component Classes” and Rooms. If it doesn’t, close the ECO dialog without executing and recheck the existence of the “ClassName” parameters and the Project Options setup done previously.
Figure 20: If not already checked, check the “ClassName” parameters.
Next, open the PCB panel (View/Workspace Panels/PCB/PCB), and set the pull-down filter to Components. Enable the Select checkbox.
The Component Classes area should show the “Ch1” through “Ch6” classes. Select the “Ch1” class and notice that the contents are components from the Ch1 circuit on the schematic (enabling Tools/Cross Select Mode in the PCB editor will also select the components in the schematic document, if opened).
Figure 21: Selecting “Ch1” reveals the components assigned to channel 1.
The components and their associated Rooms will be stacked outside the bottom right of the board area. Use Design/Rooms/Move Room to spread the Rooms apart, or simply click and drag the mouse inside the Room boundary (but not on a component body).
Setting the Channel Offset Values
The next step is crucial to this process: setting the Channel Oﬀset values. As previously mentioned, the Copy Room Formats function will only find like components whose Channel Oﬀsets match. This needs to be done manually.
Using the PCB panel as mentioned above, make sure that the “select” checkbox is enabled, then select the “Ch1” class. Next, open the PCB List panel (View/Workspace Panels/PCB/PCB List) and set the top filter to Edit selected objects Include only Components.
Figure 22: Set the filter in the PCB List to Edit selected objects Include only Components.
Sort the list by the reference designator by clicking the “Name” field header. C1 should now appear at the top of the list. Click in the “Channel Oﬀset” cell for C1, type a 0 (zero) and hit Enter. This will set C1’s Channel Oﬀset value to 0 and bring you down to the next component (D1). Type 1, then hit Enter and continue down the list, until all components are sequentially numbered.
Figure 23: Set the Channel Oﬀset values manually to sequential numbers.
Leaving the PCB List panel open, return to the PCB panel and select the “Ch2” class. The components from that class should now populate the List panel. Again, sort the list by reference designator by clicking the “Name” field header. Sorting the components this way will ensure
that the Channel Oﬀset values will be the same for the matching components in each circuit. Use the same Channel Oﬀset values as for the Ch1 components, as in Figure 24.
Figure 24: Continue for the rest of the channels.
Be sure to start numbering at 0 and continue sequentially. Copy Room Formats can deal with non- sequential values, but it will display a warning during the process, so it’s best just to avoid it in the first place.
Repeat this process until the Channel Oﬀsets for all 6 groups have been set. Being able to type directly in the List panel makes this process quick; it takes just seconds to set all the values. For larger circuits, it may be helpful to point out that external data can be pasted to multiple cells at once. This means that, for example, a spreadsheet can be used to quickly create a long column of integers: enter a 0 in a cell then CTRL+drag the corner handle to auto-increment. Copy the cells in the spreadsheet, select multiple cells in the Altium Designer List panel, then right-click and select Paste.
The last thing that needs to be done before laying out the circuit is to create the Design Channel Class in the same manner that was done for the multi-sheet method. Go to Design/Classes, right-click the “Design Channel Classes” group, select “Add Class,” and rename it “Circuit_2.” Select “Ch1” through “Ch6” and move them to the Members list. Close the dialog.
Figure 25: Add the channels to the Members list.
Layout and Copy Rooms
Locate the “Ch1” Room and move it into the board area. Click to select the Room and use the sizing handles to make it a small square or rectangle. Place Ch1’s components inside the Room and route the connections. The VCC and GND nets were left as fanout vias here.
Figure 26: Here is the circuit after moving it to the Printed Circuit Board.
Now, all that’s left is to use the Copy Room Formats exactly as was done the multi-sheet method on page 6 above. Go to Design/Rooms/Copy Room Formats. Click the “Ch1” Room as the Source, then click any one of the remaining Rooms as the Destination. Since they are all part of the same Channel Class, the system will consider all of them as valid targets for the placement and routing data. See Figure 27.
Figure 27: The final step is to use the Copy Room Formats.
In the Confirm Channel Format Copy dialog, notice that all six Rooms are presented. Ensure that the Apply To Specified Channels checkbox is enabled, and the Copy checkboxes are enabled for all of the Rooms. Click OK to run the process. The remaining five Rooms should now be placed and routed exactly like the first Room.
Note: If a Channel-Oﬀset Errors dialog pops up, it’s most likely because the oﬀset value changes made in the Setting the Channel Oﬀset Values section above were not done correctly. Check them over again.
The Rooms can now be moved into place. This can be done manually by dragging them, or by using Design/Rooms/Move Room. Additionally, there’s an automated function to arrange them evenly in a grid pattern. To run this process, first select all of the Rooms as shown in Figure 28.
Figure 28: Before arranging, select all six Rooms.
Then, as shown in Figure 29, go to the Design/Rooms/Arrange Rooms menu and set the number of columns and rows needed (in this case, 2 rows of 3 columns). Other options are available to control Room ordering, location, and spacing:
Figure 29: Next, using the Design/Rooms/ Arrange Rooms menu, set the number of columns and rows needed 2x3.
The result is a neatly spaced grid of Rooms, illustrated in Figure 30.
Figure 30: The Rooms have been automatically arranged neatly in a grid.
MAKING CHANGES TO THE PCB DESIGN LAYOUT
When changes are necessary to the circuits in your schematic, there are a few issues that must be dealt with to keep the synchronization that has been created in the previous examples.
First, when adding components to the repeated circuits using the single-sheet method, make sure that the “ClassName” parameter is added, and that their values are set properly (Ch1, Ch2, etc.). New components will have to have their Channel Oﬀset values set via the PCB List panel, as was done initially.
Regardless of the method used (single-page or multi-page), passing design changes from the schematic to the PCB may have an eﬀect on the Channel Oﬀset values. There are a few diﬀerent problems that may arise here: repeated oﬀset values for diﬀering components, skipped values in the sequence, etc. In any case, after making any sort of change it’s important to load the repeated channel components into the PCB List panel and inspect the Channel Oﬀset values to make any necessary changes.
Also, regardless of the method used, the synchronization process will attempt to remove the manually-created Design Channel Class. That change should be disabled during the ECO, shown in Figure 31.
Figure 31: Uncheck the box for Remove Channel Classes.
Once you’ve completed the ECO and performed the necessary placement and routing changes to the base Room, replicating that change across the other Rooms is as simple as rerunning Copy Room Formats, as was done initially.
Even after learning the above processes, it still may be helpful to have a checklist nearby to ensure that you don’t miss any steps.
Flat Design Using Multiple Sheets
- In SCH Inspector: Select, copy and paste the circuit from the source sheet to the target sheet(s)
- Annotate reference designators, ensuring that multi-part components are unique to each sheet
- In the Class Generation tab of Project Options, enable Component Classes and Generate Rooms for all sheets that have the repeated circuit
- In PCB: Import the design as usual. Move one Room to the PCB, then place & route the components in that Room
- In Design/Classes, create a Design Channel Class and add to it the Component Classes that were auto-generated for each sheet that has the repeated circuit
- Use Design/Rooms/Copy Room Formats
Flat Design Using a Single Sheet
- In SCH Inspector: Select the circuit and use Edit/Rubber Stamp to replicate the circuit
- Annotate reference designators
- Use Tools/Parameter Manager to add the “ClassName” parameter to all components
- Select circuits individually and set the unique “ClassName” parameters (“Ch1”, “Ch2”, etc.) using the PCB Inspector
- In the Class Generation tab of Project Options, disable Auto-Generated Component Classes, and enable User-Defined Component Classes and Room generation
- In PCB: Import design as usual
- Open the PCB panel in Components view and enable Select mode
- Select Component Class for first channel
- Open the PCB List panel in “Edit Selected Objects” mode
- Sort the components list by reference designator, then set the Channel Oﬀset values for all components sequentially starting at 0
- Go back to the PCB panel, select the next Component Class and repeat the Channel Oﬀset value step. Do this for all channels.
- In Design/Classes, create a “Design Channel Class” and add the Component Classes for the repeated channels
- Move one Room to the PCB, then place and route the components in that Room
- Use Design/Rooms/Copy Room Formats