NAD 3030 complete rebuild

Jump to Latest
#162
Goldie99 said:
Anytime you make a mistake, just use the 'undo' but to undo it, multiple times if necessary.

To delete all tracks, just select the main Edit menu, select 'Global Deletions', choose what to delete, e.g., Tracks, and press OK.
Click to expand...
I just cant see how this is going to be possible as there are far to many crossovers.Ive tried moving things around and i already have(without using SMD components) using the smallest resistor), but that then just causes another issue with another component
If i could draw the tracks manualy as per the orihginal board it could be done

Its a very frustrating programme.I get loads done, then find i have to move a component, spin it etc, but the tracks dont move with it when i move it

Im not sure its going to be possible to do it TBH
 
#163
You have to stop thinking of the 'ratsnest' lines as tracks - they are not, they just show you the 'nets'. If you're trying to rotate & move parts to avoid those crossing, forget it, it won't help. Just work your way thru' and they'll vanish / resolve themselves as your layout evolves.

I can assure you it is possible, I've worked from the pcb layout you posted in post #141 and, after correcting the schematic (as it was at that point), generated a complete pcb layout within an hour or so last night - it needs plenty of trivial adjustments / tidying, and modifications to the main terminal connection points (to fit the NAD main pcb), but the tracks, ground plane, and jumper, are essentially all fine for the present stage. You're welcome to try reproducing this layout, but I can't describe how to do it any better - just ignore the blue line (that was placed just as a 'reminder' for me).


First-Pass Layout.jpg
 
#167
Goldie99 said:
Not quite sure what you mean by 'manually place by hand' - the tracks should all be routed by hand, except, in this case there is one place where an external wire link has to be added which I was going to come to later (it connects one end of R409 to one end of C424). As far as I can see, that's the only one which should be needed if you've followed the NAD manual routings. You can actually see it on the NAD diagram, and it's the white insulated link in the pcb photo.

View attachment 1401666

View attachment 1401667

A lot of the pcb 'snippet' you just posted looks ok (not all...), but before you go any further maybe you could post a thumbnail of the entire pcb - it'll be easier to see if you're making any general mistakes, that'll be easier to fix now than later.

Two points worth mentioning at this point:

(1) For the various ground connections - we'll add a 'ground plane' to the back of the pcb (so the entire back surface becomes 'ground').
  • select the bottom copper layer of the pcb (on the RHS of the pcb screen you have the layers list, just select B.Cu - that just means whatever tools you use now will be used on the bottom copper layer)
  • select the 'Add Filled Zone' tool, and then draw a rectangle on the pcb which fills almost the entire surface of the pcb (you click each corner of the rectangle going around, and end up back at the starting point) - it'll look like a blue rectangular outline. That's created a 'zone' on the bottom layer.
  • press the letter 'B' - that'll 'fill' the zone with copper. It should add 'hatching' to the rectangular outline
  • to view the 'zone', you can use the 2 buttons on the LHS of the screen called 'Draw Zone Fills' or 'Draw Zone Outlines' (just toggle to whichever is needed at the time
  • finally, to make the new zone into a 'Ground Plane', 'Left click' any point on the zone outline to highlight it, then 'Right click' and select 'Properties' - you should see 'B.Cu' ticked as the active layer - now select '/GND' from the list of available 'nets' - just leave the rest of the entries on their default settings and click OK. That assigns the zone to be part of the GND net.
  • 'Left click' away from the pcb surface (to deselect the zone) and press 'B' again.

Note - All of the component terminals which connect to ground (/GND) are now directly connected to /GND via their solder pads, and a bunch of the ratsnest lines will have disappeared (that's why I said ignore the ground connections before).
Until now, everything you've done will have been on the Front Copper (F.Cu) layer (hopefully), but now there's 2 copper layers, so be sure to always select the layer you want to work on... that will apply to the silkscreen layers as well later.

(2) For the wire link - one of the easiest ways I've found is just to add a 'jumper' to the schematic, as follows:
  • insert a 'jumper' between R409 & C424 (you'll find jumpers listed in the components lists) as shown below
  • annotate the schematic again (so 'JP1' gets added to the annotations)
  • add a 'footprint' for the jumper - I used "Connector_Wire:SolderWire-0.5sqmm_1x02_P4.6mm_D0.9mm_OD2.1mm"
  • switch to the pcb screen, and 'update' the pcb for changes to the schematic - so the jumper is added as a new component (it's the 2 square 'terminal pads' in the pcb snippet below, above R409 & C424)

That'll add a 2 terminal 'jumper' to be inserted onto the pcb - it needs to be placed in such a way that one terminal can be directly connected to R409 with a new pcb track, and the other terminal can be directly wired to the appropriate terminal of C424.

Note - You will need to 'edit' the footprint to space the 2 terminals of the jumper further apart (you can see from the footprint name that they're only 4.6mm apart in the std. footprint) - that can be done just on the pcb screen (right click, edit footprint, etc.) and saved without affecting the library footprint. It's a useful exercise in itself, for working with footprints (do it off to the side of the pcb screen to avoid accidentally interferring with the pcb layout).


View attachment 1401692 View attachment 1401693

Just an aside - you can 'toggle' (hide) the various layers on/off as needed, so try toggling the front and back fabrication layers off, it'll be easier to see for routing.
Click to expand...
(1) For the various ground connections - we'll add a 'ground plane' to the back of the pcb (so the entire back surface becomes 'ground').

  • select the bottom copper layer of the pcb (on the RHS of the pcb screen you have the layers list, just select B.Cu - that just means whatever tools you use now will be used on the bottom copper layer)
I cant actualy see the menu you are refering to for the layers list
1735891079277.png
 
#170
Goldie99 said:
Not quite sure what you mean by 'manually place by hand' - the tracks should all be routed by hand, except, in this case there is one place where an external wire link has to be added which I was going to come to later (it connects one end of R409 to one end of C424). As far as I can see, that's the only one which should be needed if you've followed the NAD manual routings. You can actually see it on the NAD diagram, and it's the white insulated link in the pcb photo.

View attachment 1401666

View attachment 1401667

A lot of the pcb 'snippet' you just posted looks ok (not all...), but before you go any further maybe you could post a thumbnail of the entire pcb - it'll be easier to see if you're making any general mistakes, that'll be easier to fix now than later.

Two points worth mentioning at this point:

(1) For the various ground connections - we'll add a 'ground plane' to the back of the pcb (so the entire back surface becomes 'ground').
  • select the bottom copper layer of the pcb (on the RHS of the pcb screen you have the layers list, just select B.Cu - that just means whatever tools you use now will be used on the bottom copper layer)
  • select the 'Add Filled Zone' tool, and then draw a rectangle on the pcb which fills almost the entire surface of the pcb (you click each corner of the rectangle going around, and end up back at the starting point) - it'll look like a blue rectangular outline. That's created a 'zone' on the bottom layer.
  • press the letter 'B' - that'll 'fill' the zone with copper. It should add 'hatching' to the rectangular outline
  • to view the 'zone', you can use the 2 buttons on the LHS of the screen called 'Draw Zone Fills' or 'Draw Zone Outlines' (just toggle to whichever is needed at the time
  • finally, to make the new zone into a 'Ground Plane', 'Left click' any point on the zone outline to highlight it, then 'Right click' and select 'Properties' - you should see 'B.Cu' ticked as the active layer - now select '/GND' from the list of available 'nets' - just leave the rest of the entries on their default settings and click OK. That assigns the zone to be part of the GND net.
  • 'Left click' away from the pcb surface (to deselect the zone) and press 'B' again.

Note - All of the component terminals which connect to ground (/GND) are now directly connected to /GND via their solder pads, and a bunch of the ratsnest lines will have disappeared (that's why I said ignore the ground connections before).
Until now, everything you've done will have been on the Front Copper (F.Cu) layer (hopefully), but now there's 2 copper layers, so be sure to always select the layer you want to work on... that will apply to the silkscreen layers as well later.

(2) For the wire link - one of the easiest ways I've found is just to add a 'jumper' to the schematic, as follows:
  • insert a 'jumper' between R409 & C424 (you'll find jumpers listed in the components lists) as shown below
  • annotate the schematic again (so 'JP1' gets added to the annotations)
  • add a 'footprint' for the jumper - I used "Connector_Wire:SolderWire-0.5sqmm_1x02_P4.6mm_D0.9mm_OD2.1mm"
  • switch to the pcb screen, and 'update' the pcb for changes to the schematic - so the jumper is added as a new component (it's the 2 square 'terminal pads' in the pcb snippet below, above R409 & C424)

That'll add a 2 terminal 'jumper' to be inserted onto the pcb - it needs to be placed in such a way that one terminal can be directly connected to R409 with a new pcb track, and the other terminal can be directly wired to the appropriate terminal of C424.

Note - You will need to 'edit' the footprint to space the 2 terminals of the jumper further apart (you can see from the footprint name that they're only 4.6mm apart in the std. footprint) - that can be done just on the pcb screen (right click, edit footprint, etc.) and saved without affecting the library footprint. It's a useful exercise in itself, for working with footprints (do it off to the side of the pcb screen to avoid accidentally interferring with the pcb layout).


View attachment 1401692 View attachment 1401693

Just an aside - you can 'toggle' (hide) the various layers on/off as needed, so try toggling the front and back fabrication layers off, it'll be easier to see for routing.
Click to expand...
ok i have found how to do this and followed your instructions
1735896099960.png
 
#171
poundy said:
I cant actualy see the menu you are refering to for the layers list
Click to expand...
You've turned the 'Appearance Manager' option OFF - it's an option in the main 'View' menu

poundy said:
one thing i noticed this morning was that you have an additional component compaired to mine-circled in white-what is this?
Click to expand...
That's C424 (the 1nf cap on the -ve (Vee) power rail)
If you mean the small square above it - that's 1 of the 2 pads of the 'jumper' JP1

It's certainly looking a lot better now, although it's difficult to see properly with all the 'fabrication layer' still visible. A couple of observations:

# You're still using 90 degree 'turns' for a lot of tracks - you should stick to straight or 45 degree turns, not 90 degrees

# Some of your capacitor footprints seem to have become smaller - that's no problem, but remember the pcb is now in the 3D real world, so make sure the relevant caps will still actually fit (dimensionally), or you might end up with pcb spaces too small for the actual caps. The footprints have to assign component areas large enough for the complete parts, not just their connections.

# You seem to have the 'ground plane' drawn OK on the bottom layer, but may have lost the board 'edge-cuts' (the physical outline of the pcb) ? or they may be 'hidden' now ? I can't tell. In any case, the ground plane should fit within the edge-cuts area. Don't forget to assign it to the main 'ground net' whatever it's called now, and to use the 'B' key to actually fill the plane with Copper and make the various connections to ground terminals (you still have some ground tracks drawn that are not needed).
 
Last edited:
#172
Next Steps

To make everything somewhat easier to read - try reducing the text size for the part designators:
# Edit Menu, 'Select All'
# Edit Menu, select ‘Text & Graphic Properties'
# Under 'Scope' – tick ‘Reference Designators’
# Under ‘Filters’ – tick ‘Filter Items by layer’ and select ‘Front Silkscreen’ as the layer
# Change the Text Width & Text height values (I’m using 0.8mm for now) and Text Thickness (0.08mm), and make ‘Visible’ the only ticked box on the right
# Click ‘Apply’, then 'OK'

All of the part designation labels (‘R401’, etc) should now be smaller - they can be done individually on the pcb page, but it's quicker / easier to do all at once.

To use a more realistic track size, we can choose say 0.5mm:
# At the top left of the screen - open the dropdown 'Track' menu
# Select 'Edit pre-defined sizes'
# Under the 'Tracks' Column, press the '+' button, type in a new value of 0.5mm track width, and then press 'OK'

You've now added a 0.5mm track width option to the project.

Now try changing all of the tracks on the pcb to 0.5mm width, they can all be done at once.
 
#174
# Look at the ground tracks in my example - from J5 & J7
# Make sure you have 'assigned' the ground plane to the main ground net (the one J5 is on), and used the 'B' key to fill the plane and connect the ground terminals.

# "What's above it ?" - no offense, but please actually read what I've already written
Goldie99 said:
That's C424 (the 1nf cap on the -ve (Vee) power rail)
If you mean the small square above it - that's 1 of the 2 pads of the 'jumper' JP1
Click to expand...
 
  • Like
Reactions: poundy
You must log in or register to reply here.
Top Bottom