PCAD 2006 PCB Layout Question About Positioning Parallel Circuits

[bostonman]

I use PCAD 2006 and a design I have in mind is using identical circuits.

Usually when I see PCBs with identical circuits, the components are all in identical places. Similarly, at my old job where they used PCAD, I saw the same layout when identical circuits were used.

Normally, as with other PCB software, I'd create the schematic first, export the netlist, and then manually move all the components in place.

I'm wondering if a way exists so I can layout circuit A in the PCB portion of the design, and then mimic the component placement traces, etc... for circuit B, C, etc...?

I'm assuming create circuit A in the schematic, export the netlist, move the components on the PCB, and then return to the schematic to copy circuit A and paste it to create circuit B, C, etc... but uncertain how to incorporate this into the PCB portion so the components are all placed identically.

[nigelwright7557]

You could try copying the circuit in the pcb end ?
Then when finished back annotate to the schematic.

[xvr]

A long time ago I made a special utility for this purpose. It still run on Win11 (I'd test it right now).
Here is read.me from it:

hrgr.exe is a DBX (P-CAD) utility for grouping components on a PCB according to the hierarchy in Schematic.

What hrgr.exe does.

P-CAD supports a very convenient feature in the schematic called Modules (Utils -> Module Wizard).
Unfortunately, this support remains in the schematic. When moving to the PCB, P-CAD washes its hands of it and leaves the user to their own devices, to figure out the modules it generated. It's quite reasonable that if a schematic contains duplicate parts, the components that comprise them will also be arranged similarly on the PCB.

Unfortunately, P-CAD doesn't know about this, and apparently never will. However, it can be taught.
------------------------------------

How to use hrgr.exe.

The utility consists of two screens.

The first screen specifies the set of components that form the grouping units (most likely, these will be modules generated by P-CAD by executing the Utils->Resolve Hierarchy command, but these could be any other sets of components).

Component groups are displayed in the Group Selector table. Each row corresponds to one component group. Components
located in the same column of each group will be arranged uniformly within all groups. The groups themselves will be arranged
in a matrix.
The second screen is where you actually group components. Here you can also set the number of rows or
columns in the group matrix, as well as the gap between groups. The second screen also offers additional options (see below).

How to use:
1) Launch SCH and PCB (you can use just PCB, but some utility functions will be unavailable).
2) Load the schematic into SCH AFTER executing the Utils->Resolve Hierarchy command.
3) Load the PCB with components into PCB (you can use a pristine board, directly from Utils->Load Netlist, or one that has already been edited).
4) In the utility, click Load SCH (if you don't have SCH, click Load PCB).
All components in your design will appear in the list on the right.
5) Create groups. This can be done in several ways:
a) Drag and Drop from the component list to the Group Selector table. Drag and Drop also works within the table, and from the table
to the component list (to remove components from groups). During D&D, the table highlights locations where
a component can be dropped. (When the table is full, the start of D&D may be somewhat slow—please be patient.)
b) Add an entire row to the table. You can add selected (or highlighted) components from the design
(the Add Highlighted button), or selected components from the list on the right (check boxes in the list and the Add Selected button).
The first row in the table can be arbitrary; subsequent rows must consist of similar components.
(Components must have matching types, values, libraries, and connections to other components from the first row.)
Therefore, when adding the second and subsequent rows, various unexpected situations may arise:
1. The number of added components is not equal to the number of components in the first row - hrgr will return an error.
2. The components do not match the components in the first row - hrgr will return an error and indicate which component it failed on (this does not mean that other components are compatible, it only means that THIS component is NOT compatible).
3. Components can be laid out in several different ways - hrgr will list all the layout methods and prompt you to
select one.
c) Automatically generate a list of components from modules in SCH (Fill By Sheets button). If hrgr detects more than one macro/module set in a design, it will prompt you to select the required set (from the list of Shchet names in the design). This method of populating the group list first clears the entire table contents and then repopulates it.
After populating, you can edit the resulting list (see methods a and b).
If an extra element was added to a group during the process, it can always be deleted by dropping it onto the list of elements or
by selecting it in the table (using the keyboard) and pressing the Delete key.
NB: You can restart the process at any time by restarting hrgr or by clicking the Clear Design button. The first method
is preferable, as the second is sometimes glitchy – when populating the group table using methods b and c, 'illegal' components sometimes appear.

6) After populating the groups, switch to the second screen (Place Groups). This screen shows a list of groups, including the main group (highlighted in the list). The components of this group form the template for arranging the remaining groups.
There are also two tabs at the bottom of the screen: Place (the actual placement) and Others (auxiliary features).
7) Place the main group in the PCB.
Specify where the main group will be located in the placement grid (Place Group -> Placement Grid Configuration -> one of the corners or Unrelated. In the latter case, the main group will not be in the placement grid, and the lower-left corner of the grid will need to be specified explicitly in the X and Y fields.
9) Specify the number of columns or columns.
The origin in the group matrix and the gap between group edges (Gap) or the distance between group centers (Delta). All coordinates are aligned to the current grid value in the PCB (if a relative grid is specified, the
grid origin value is also incremented).
10) Click Place - hrgr duplicates the placement (taking into account component flips and rotations) of the main group's components in all other groups.
If you moved (or otherwise modified the design), click Update - hrgr will recalculate the design and
recalculate the coordinates.

Additional features (Others tab):
1) Group Current - allows you to remove components of the selected group from the design and place them in a separate location.
Specify the coordinates of the lower left corner to place the components and the desired gap between them, and click the Group button.
2) Highlight Current/Unhighlight/Highlight Automatic - Allows you to highlight a group of components, or automatically
hover a group, when moving the selector in the Main Group list. (With automatic highlighting, it is not recommended to
jump to the Main Group too quickly - this may cause problems.)
--------------------------------

The hrgr utility works with P-CAD2006; I haven't tested it with other utilities (it may or may not work).

--------------------------------
Disclaimer: This utility is supplied AS IS, with all bugs and imperfections. The author is not responsible for the consequences of using the utility,
for the consequences of using P-CAD, for Altium's mistreatment of P-CAD, for Altium's pricing,
for Altium's position on the NASDAQ, for the dollar exchange rate (including the Australian dollar), for the Dow Jones Index, etc., etc.

[bostonman]

You could try copying the circuit in the pcb end ?
Then when finished back annotate to the schematic.

That was one of my thoughts. In the board at my old job, circuit 1 had components as ref des 1xx, circuit 2 as ref des 2xx, etc... Then the PCB had each circuit in perfect alignment with each other. It's possible circuit 1 was laid out in the PCB and copied/pasted to circuit 2, then the net list was sent to the schematic to incorporate circuit 2, etc...

I think having every circuit in alignment with each other is good so noise is equal in all circuits, but it's also neater and provides for easier troubleshooting later.

Thanks for the file, I'll give it a try as well.

I believe PCAD has auto placement or whatever and tinkered with it once if I remember correctly. Wasn't sure if my placement desires was something simple that could be automated or just required some hands on tinkering.

[temperance]

for Altium's mistreatment of P-CAD,

I like that one. I once told an Altium sales rep to have a close look at PCAD and see how PCAD works and toss Altium into the garbage.

[Doctorandus_P]

Maybe it's time to consider an upgrade?

In KiCad, this is just "built in". You draw your schematic on a single sheet, and then add multiple instances of that sheet in the schematic. This ensures that even if you change the schematic, you only have to modify one instance, and the other instances will always be the same. Similar for the PCB. You layout one instance, and for the other instances, you just define the location and KiCad does the rest for you.

I never used P-Cad. I guess it must have been better than altium, and that is probably why they killed it.
https://en.wikipedia.org/wiki/P-CAD

The 2006 version was the last and that is quite a long time ago. KiCad is FOSS, and thus free to use, (or try it out for an indefinite period). It will also never ever do vendor lock in or other nasty things that are designed to extract money from their customers. KiCad implements features that their users want, because for a big part it depends on voluntary donations from their users. Vote with your money if you wish. It's also actively developed, with around 60 new features every year.

[bostonman]

Ironically I didn't realize a Wiki page existed about them.

It may be time to switch, but my goal is usually to learn software used in industry (i.e. Altium), but obtaining it for personal use isn't worth the cost; unless they have a home user one, but those are usually too restricted and not worth it.

KiCAD is very popular from what I've seen, so it's worth learning. It's just that the few PCBs I layout (maybe three in the last five-years) forces me to stick with what I know.