Protel 98SE netlisting problem

Hello,

I have an application where the schematic is dictated by the layout design. I have manually routed my board and I am trying to find a way to efficiently assign my traces/pins net names. The reason for this is that design rules are not enforced unless the trace/pin/component has been assigned a net. This board contains 375 nets, so I would very much like to use the DRC.

So far, my only success in assigning nets has been to go into the netlist manager and creating nets manually and assigning them their respective pins. So far this has shown to be an extremely time-consuming method of creating nets in a layout. In addition, after nets are created via Netlist Manager, the trace that I manually drew lights up as an error as the actual trace itself is not assigned the net respective the pin it is connected too.

Also, another method I have tried w/out success:
1. Create netlist text file from connected copper.
2. Manually edit netnames in *.net file.
3. Load edited *.net file into pcb.

Whenever I have tried this, I get errors stating: component not found.

Any ideas?

Thanks in advance.....

Nets are created from the schematic. There is no way except manually writing a netlist to do otherwise. A PCB layout is the physical realization of a schematic, so the statement that the schematic is layout driven is not possible by definition.

If you mean that you don't know pin assignments or channels until you do the layout, you give arbitrary pin assignments in the schematic until you do the layout -then you back-annotate the schematic to correct the assignments, and generate an accurate netlist from the revised schematic.

All that having been said - if you are getting error messages about components not existing, it is because you have failed to place the component definition statements at the beginning of your manually produced netlist. You may also have screwed up the netlist punctuation somewhere. Look carefully at how brackets and parentheses are used in the netlist.

A manually written netlist must define each component, then define each node on the board - that means every pin must be accounted for.

House_Cat, thank you for your very knowledgeable reply.

Nets are created from the schematic. There is no way except manually writing a netlist to do otherwise. A PCB layout is the physical realization of a schematic, so the statement that the schematic is layout driven is not possible by definition.

If you mean that you don't know pin assignments or channels until you do the layout, you give arbitrary pin assignments in the schematic until you do the layout -then you back-annotate the schematic to correct the assignments, and generate an accurate netlist from the revised schematic.

Click to expand...

In my application, it is the layout that determines the pin assignments, which determines the schematic.=)

All that having been said - if you are getting error messages about components not existing, it is because you have failed to place the component definition statements at the beginning of your manually produced netlist. You may also have screwed up the netlist punctuation somewhere. Look carefully at how brackets and parentheses are used in the netlist.

A manually written netlist must define each component, then define each node on the board - that means every pin must be accounted for.

Click to expand...

I figured out what my error was in my manually scripted netlist. The "designator" names for each component had a space in it and was causing it to be read wrong when loading the netlist into Protel.

After reading the first part of your response, I realize now that the most efficient way of attacking this application is to assign net aliases (I'm using Capture) to the known pins in the schematic. Then load the netlist into Protel, and then manually route the traces to the desired pins.

After that I still need to back-annotate the schematic, like you said. Whew.....
Its funny, when my girlfriend asks what I do at work, I just tell her I connect dots, hehe.

Thanks again for your reply House_Cat!