Can you use CS without a schematic ?

[mikeselectricstuff]

Just started looking  at CS - been using PCAD for many years.
My normal design flow does not start with a schematic ( there are many reasons for this - will probably do a vid sometime!).
I put down parts & pads, create nets within the PCB layout by rubberbanding between , then place & route.
I've been playing around with CS and can't immediately see a way to work like this - I've not found any way to create nets within the PCB editor.
Is this workflow possible in CS?

[trophosphere]

It is possible to create nets within the PCB editor.

With a blank pcb file opened, go to the ribbon menu and navigate to Tools>Netlist>Edit Nets... This will open up a dialog box that will contain all nets in your pcb. Hit the 'Add" button and then fill out the needed information - e.g. net name, trace width, and via sizing. Click the "Okay" button and the newly created net should then appear in the first list box.

Assigning nets to pads can be done by double-clicking on the pad of interest to get into the properties dialog box and then selecting the net under the properties section.

[mikeselectricstuff]

It is possible to create nets within the PCB editor.

With a blank pcb file opened, go to the ribbon menu and navigate to Tools>Netlist>Edit Nets... This will open up a dialog box that will contain all nets in your pcb. Hit the 'Add" button and then fill out the needed information - e.g. net name, trace width, and via sizing. Click the "Okay" button and the newly created net should then appear in the first list box.

Assigning nets to pads can be done by double-clicking on the pad of interest to get into the properties dialog box and then selecting the net under the properties section.

I'd figured out the latter after importing a PCAD design, but that whole process is tedious enough to be a complete dealbreaker.

[Someone]

Its possible to turn off the short circuit checking and draw PCBs freehand without a netlist, I've done this in Protel for some simple designs that are more constrained in shape/position than in PCB design rules. Just to check for you I fired up AD and put some parts down, you can freely draw in connections between parts but the "Create Netlist From Connected Copper" command doesn't seem to function but "Configure Physical Nets" did assign nets to all the connected copper and then the design rules all run normally. You could very well run "Configure Physical Nets" periodically while routing and do a board entirely without a schematic and still end up with a good coverage of interactive and offline design rules.

[mikeselectricstuff]

I don't often want to draw without a netlist (although this can be useful for things like large arrays), I want to create the netlist quickly and easily within the PCB editor.
With PCAD, I go into  "place connection" mode, drag a connection line between pads - if it's a new net it pops up a dialog with a default net name (NETxxxx) , which I can either edit or just hit enter to use the default.
I can also right-click on a pad and do "add to net" from a list of the nets in the design.
As for DRC, it can manually route using the design rules so you generally end up with most rules met. Subsequent dragging of parts & tracks can break the rules but you can just run manual DRC which tags issues for manual fixing. ,

[tautech]

I don't often want to draw without a netlist (although this can be useful for things like large arrays), I want to create the netlist quickly and easily within the PCB editor.
With PCAD, I go into  "place connection" mode, drag a connection line between pads - if it's a new net it pops up a dialog with a default net name (NETxxxx) , which I can either edit or just hit enter to use the default.
I can also right-click on a pad and do "add to net" from a list of the nets in the design.
As for DRC, it can manually route using the design rules so you generally end up with most rules met. Subsequent dragging of parts & tracks can break the rules but you can just run manual DRC which tags issues for manual fixing.

Altium isn't much different, a trace or pad double clicked will show Properties in which nets can be assigned.
A free pad or trace Properties will show as "No Net" within a netlist box and existing nets can be assigned to your new pad or trace.
I've used this on the odd occasion when library parts haven't linked correctly and also when you need a quick fix to a routing problem with multi gate logic packages and aren't worried about updating the schematic as you can do it later from the finished PCB.

[Someone]

I don't often want to draw without a netlist (although this can be useful for things like large arrays), I want to create the netlist quickly and easily within the PCB editor.
With PCAD, I go into  "place connection" mode, drag a connection line between pads - if it's a new net it pops up a dialog with a default net name (NETxxxx) , which I can either edit or just hit enter to use the default.
I can also right-click on a pad and do "add to net" from a list of the nets in the design.
As for DRC, it can manually route using the design rules so you generally end up with most rules met. Subsequent dragging of parts & tracks can break the rules but you can just run manual DRC which tags issues for manual fixing.

Altium isn't much different, a trace or pad double clicked will show Properties in which nets can be assigned.
A free pad or trace Properties will show as "No Net" within a netlist box and existing nets can be assigned to your new pad or trace.
I've used this on the odd occasion when library parts haven't linked correctly and also when you need a quick fix to a routing problem with multi gate logic packages and aren't worried about updating the schematic as you can do it later from the finished PCB.

Adding pins to nets manually is useful for exposed pads or odd connectors with many mounting pins that you want to use as conductors/vias. But back on the OP there isn't an easy way to create named nets (that I know of or could find), seems like Mike has a very specific workflow in mind which isn't possible as far as I can see.

[tszaboo]

Altium's normal design flow was always SCH->PCB. You will save yourself from a lot of headaches if you follow this. I believe the correct way is to set the pads to a net, and then just connect them together. I think you have to select the pads you want to connect, open the PCB inspector panel, and then enter a net name to the net. But be prepared that this will make your life very hard, with a lot of issues.
I'm not sure if CS has pin swapping support, but I assume that is one the reason you want to do it this way.

[mikeselectricstuff]

It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.

If you're doing a PCB with >1K LEDs (on 2 layers) , this stuff matters rather a lot. 

[tszaboo]

It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.

If you're doing a PCB with >1K LEDs (on 2 layers) , this stuff matters rather a lot.

Yes, in CS it will be a pain in the arse. In Altium you make a SCH with a single LED or some LEDs, place multiple SCHs as a sub sheet,a so called "room" is created, then you route it, and then just "copy room" so the routing on all the rooms are the same. CS... forget it, that would be productive.
Also, there is the SCH list, where you can just copy from excel (or whatever) the location info for a component or a net. That is gone in CS.
I'll try to think something, but I only had CS trial license. Did you buy it or just trying?

[mikeselectricstuff]

It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.

If you're doing a PCB with >1K LEDs (on 2 layers) , this stuff matters rather a lot.

Yes, in CS it will be a pain in the arse. In Altium you make a SCH with a single LED or some LEDs, place multiple SCHs as a sub sheet,a so called "room" is created, then you route it, and then just "copy room" so the routing on all the rooms are the same. CS... forget it, that would be productive.
Also, there is the SCH list, where you can just copy from excel (or whatever) the location info for a component or a net. That is gone in CS.
I'll try to think something, but I only had CS trial license. Did you buy it or just trying?

They gave me a freebie - Dave emailed me to let me know they were desperate for bloggers etc. to look at it.
With a few small additions it could be a good solution - I don't think there's anything fundamentally broken, just that they'd not considered a layout-centric design entry method.
I think a reason that PCAD originally made this easy is that you used to be able to buy PCB seperate from schematic.
 

[tszaboo]

Creating a component - from the PCB section you want to multiply - could work. Only your Pick & Place file and your BOM will need some work afterwards.
I also see "create netlist from connected copper" in the netlist menu. Basically turn off online DRC, connect what you want, create netlist, update SCH, enable DRC. Maybe you need to go to PCB rules and disable the short circuit rule for the time.

[free_electron]

place LINE

wire up board

then pull a netlist from the board.

[mikeselectricstuff]

place LINE

wire up board

then pull a netlist from the board.

I also see "create netlist from connected copper" in the netlist menu

That would be the equivalent of PCAD's "reconnect nets", which creates or merges nets based on previously placed tracks.
Just tried in CS, and it doesn't appear to work, at least not how I'd expect - after doing "create netlist" I'd expect to see teh new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

[tautech]

I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?

[mikeselectricstuff]

I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?

Yes - if any uncommitted pad intersects an uncommitted track or polygon, a new net is created with a name of the form "NETxxxx" where xxx is an incrementing number. If an uncommitted pad intersects a track that has a net, that pad is added to that net.
Class would be whatever is the default.

[tautech]

I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?

Yes - if any uncommitted pad intersects an uncommitted track or polygon, a new net is created with a name of the form "NETxxxx" where xxx is an incrementing number. If an uncommitted pad intersects a track that has a net, that pad is added to that net.
Class would be whatever is the default.

Ah, now I see why you liked PCAD for your work flow. 

[Someone]

It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.

I've not had many problems with the "smart" pasting merging/reassigning nets based on what you're dropping it onto.

I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?

Yes - if any uncommitted pad intersects an uncommitted track or polygon, a new net is created with a name of the form "NETxxxx" where xxx is an incrementing number. If an uncommitted pad intersects a track that has a net, that pad is added to that net.
Class would be whatever is the default.

If you don't mind the nonsense net names of "NewNetxxx" then the above workflow using the "Configure Physical Nets" works, but you'll have to manually add pads if you want rats nests along the way, the rats nest will appear on routed nets after each "Configure Physical Nets". Renaming of nets automatically propagates so you can add some readable names as needed.

Once there is a named net on some copper you can't connect any of the "No Net" primitives to it with normal interactive routing turned on, turn off the push/avoid routing and you can flow copper anywhere you like and nets will merge automatically though the "Configure Physical Nets" along with allocating pads and copper.

This is all with AD, some or any of the options might be missing from CS.

[free_electron]

place LINE

wire up board

then pull a netlist from the board.

I also see "create netlist from connected copper" in the netlist menu

That would be the equivalent of PCAD's "reconnect nets", which creates or merges nets based on previously placed tracks.
Just tried in CS, and it doesn't appear to work, at least not how I'd expect - after doing "create netlist" I'd expect to see teh new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

once youcreate such a netlist you need to push it. do a net-clean all. ( dont know if it exists in CS but it does in big altium.)