Shop OBEX P1 Docs P2 Docs Learn Events
Diptrace help please? — Parallax Forums

Diptrace help please?

RforbesRforbes Posts: 281
edited 2014-06-26 19:35 in General Discussion
Heya all,

I'm just getting started using DipTrace and I am trying to figure out what I'm doing wrong here.

My attachment is the schematic that I'd like to turn into a board with 2 signal layers, a ground plane and a power plane (3.3v)
The schematic has no errors, and when I use it to create a PCB it lays everything out fine.

However- it routes traces for Vcc and Gnd to each component on the signal layers.

Can someone explain what I need to do to make the Vcc and Gnd connections connect directly to a 3rd and 4th plane (Vcc and Gnd?) This should eliminate the traces.

Thanks in advance!
Robert
zip
zip
test.zip
7K

Comments

  • PublisonPublison Posts: 12,366
    edited 2014-06-25 06:54
    Are you using the Freeware version?

    It is limited to 2 signal layers. I can't find any reference to Ground and Power layers.
  • RforbesRforbes Posts: 281
    edited 2014-06-25 07:09
    @Publison- Yep, using the freeware version. When I create the pcb, I can use the layer manager to add layers- I have a choice of signal, non-signal or plane type for the layer. I sort of thought I could add a new plane layer, and connect all the Vcc pins to it. Same thing with ground. I' just not sure how to do it or if the freeware supports that ? A plane isn't a signal layer, so.... ?
  • Duane DegnDuane Degn Posts: 10,588
    edited 2014-06-25 07:21
    Diptrace says "Unlimited plane layers (power, ground) for all editions. " so I'd think you should be able to add power and ground planes with the free version.

    I got a "wrong format" error when I tried to open the file. I have a Standard license myself so I'd think it would be able to open a file created by the free version. The version # on mine is 2.2.0.2. I wonder if I need an update in order to open your file?
  • RforbesRforbes Posts: 281
    edited 2014-06-25 07:25
    Duane- Uhh... no idea bud. I have a whole 2 hours using dip trace now- just downloaded it yesterday. My version is 2.4.0.0 and I have no option to save as an older version. Just a regular ole .dch file for the schematic and a .dip for the board layout.
  • PublisonPublison Posts: 12,366
    edited 2014-06-25 07:42
    I can open it with 2.4.0.1 after upgrading and rebooting.

    I've not done Power/Ground planes with this software before. Time to learn! :)
  • RDL2004RDL2004 Posts: 2,554
    edited 2014-06-25 08:24
    Go to Google and search:

    diptrace how to multi layer

    First result will probably be a post on the Diptrace forums that has a response from their tech support guy Alex.

    If that doesn't work I'd probably look for more help on the Diptace forums.
  • Dave HeinDave Hein Posts: 6,347
    edited 2014-06-25 08:39
    I've only done one PCB with diptrace, so I don't have a lot of experience with it. However, I think you could do a 2-layer board with copper pours for ground on one layer and power on the other layer. I did copper pours with ground on both layers on my board. Click on "Objects" and then "Copper Pour". You then specify an area on the board where you want the copper pour.
  • Alex.StanfieldAlex.Stanfield Posts: 198
    edited 2014-06-25 15:46
    Rforbes wrote: »
    Heya all,

    I'm just getting started using DipTrace and I am trying to figure out what I'm doing wrong here.

    My attachment is the schematic that I'd like to turn into a board with 2 signal layers, a ground plane and a power plane (3.3v)
    The schematic has no errors, and when I use it to create a PCB it lays everything out fine.

    However- it routes traces for Vcc and Gnd to each component on the signal layers.

    Can someone explain what I need to do to make the Vcc and Gnd connections connect directly to a 3rd and 4th plane (Vcc and Gnd?) This should eliminate the traces.

    Thanks in advance!
    Robert

    First the free version is "All features and libraries, 300 pins and 2 signal layers, non-profit use only"

    Second, even if you could do 4 layers, are you sure you want that? It's more expensive and you will not be able to do a DIY board. Is that what you really need?

    I usually approach it in this order:
    1 - Make first attempt to define board size
    2 - Work the component placement according to schematic/connector needs
    3 - Try 1 layer routing
    4 - If after "N" attempts (depending on schematic compplexity and max board size requirements) I don't succeed then try 1 layer + jumpers on second layer.
    5 - If not possible revert to 2 layer design

    Alex
  • Duane DegnDuane Degn Posts: 10,588
    edited 2014-06-25 15:57
    As I understand it, it's common practice to have additional ground and power layers. Diptrace limits the signal layers but not the ground and power layers. I haven't used these ground and power planes in any of my own designs so I don't know how one goes about doing this in Diptrace.

    I think there are reasons to use ground and power layers other than to aid in routing paths for these traces. I believe these layers benefit PCBs by reducing noise and keeping the power clean.
  • PublisonPublison Posts: 12,366
    edited 2014-06-25 16:10
    Power and ground layers are used to reduce traces on top and bottom layers. I does help in noise situations. The downside is the cost of manufacturing and the attention to the vias feeding the planes, versus through holes.
  • RforbesRforbes Posts: 281
    edited 2014-06-25 18:00
    Alex- Very good points, and that's a good strategy. Thanks! I'd like to keep a segregated power and ground plane for managing stray capacitance and noise and such, as Dave Hein and Duane D have pointed out.

    I've only created pcb with ExpressPCB which is incredibly simple to use, and creating the power and ground planes is very straight forward. Diptrace, so far seems like it's a much better software package and incredibly useful. I wish I had more time to learn it, but for now I'm somewhat limited (hence my question.)

    The biggest advantage to having separate power and ground planes is minimized routing on the top and bottom signal planes. But the other great advantage is being able to "tap" power or ground from anywhere on the board, wherever you need it-without using real estate for the trace to get it there.

    Rick sand Dave- thanks! I'mma keep trying. It can't be that difficult. I must be overthinking it or something.

    Publison- if you figure it out, lemme know! I'll be sure to post any tidbits I figure out.
  • RDL2004RDL2004 Posts: 2,554
    edited 2014-06-25 18:32
    From the post on the Diptrace forums:
    1. Add internal layer using "Layer/ Layer setup" from main menu. Give layer name, color, plane type and assign net to the layer.
    2. Switch to the new layer and place copper pour on it. Connect copper pour to the same net as the layer. In copper pour properties dialog window, go to border tab and click on "Depending on board" and "Snap to board outline" items.

    Doesn't sound too hard, have you tried it?
  • RforbesRforbes Posts: 281
    edited 2014-06-26 04:44
    Rick-
    1. Add internal layer using "Layer/ Layer setup" from main menu. Give layer name, color, plane type and assign net to the layer.
    2. Switch to the new layer and place copper pour on it. Connect copper pour to the same net as the layer. In copper pour properties dialog window, go to border tab and click on "Depending on board" and "Snap to board outline" items.


    I just got back to my computer and tried it. Perfect! Thanks tons :)

    A few more hints and tips to go with this:

    -When you use Schematics to "Convert to pcb" you should take the following steps in order:
    1- arrange the components (manually or automatically) for the board layout.
    2- Create the power and ground planes and select the net to connect to the plane at the time of creation (this is done BEFORE using auto-route.)
    3- Perform auto-route last. For whatever reason, if you don't, it can throw some errors. Not sure why.


    I've found the following additional hints and tips to be useful
  • PublisonPublison Posts: 12,366
    edited 2014-06-26 10:29
    Glad you got it to work!

    I had zero time last night to try the suggestions. I will have zero time until the weekend. :(
  • Igor_RastIgor_Rast Posts: 357
    edited 2014-06-26 16:06
    You dont realy need to listen to me , but if your just getting into it

    USE KiCad

    Opensource , no limitations . what else need i say

    http://www.kicad-pcb.org/display/KICAD/KiCad+EDA+Software+Suite
  • NWCCTVNWCCTV Posts: 3,629
    edited 2014-06-26 19:35
    Downloading KiCad now. I do not have an immediate use for it but will play with it a little and post my results.
Sign In or Register to comment.