1. Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.
    Dismiss Notice

Setting Eagle Default Units to mm - How?

Discussion in 'Circuit Simulation & PCB Design' started by Angry Badger, Dec 8, 2011.

  1. Angry Badger

    Angry Badger Member

    Joined:
    Jun 29, 2008
    Messages:
    201
    Likes:
    8
    Location:
    Flintshire, North Wales
    Hi,

    Tried putting this in the 'eagle.scr' file under the SCH and BRD sections: Grid mm;

    but it won't allow me to save the file after entering the change - gives error code5. I suspect I'm not editing the .scr file properly.

    Can anybody help me out here please? Bonuck - are you there?

    Update: Ok, managed to save the file after changes but first had to make it a text file then save as .scr again. Didn't change the default units though.
     
    Last edited: Dec 8, 2011
  2. Sceadwian

    Sceadwian Banned

    Joined:
    Oct 27, 2006
    Messages:
    14,047
    Likes:
    141
    Location:
    Rochester, US
  3. Boncuk

    Boncuk New Member

    Joined:
    Nov 10, 2007
    Messages:
    5,382
    Likes:
    88
    Location:
    Phetchabun,Thailand
    Hi Angry Badger,

    I do not recommend to use a metric grid size in the board editor since most parts are inch-based.

    Using a metric grid and designing a board you will get a never ending list of "off grid" errors when you perform a DRC (design rule check). Additionally you'll have problems getting traces straight in to pads which then results in "angle" errors.

    Using a metric grid in a schematic is not recommendable either since the symbols are all created on an inch based grid. Using a metric grid in the schematic editor will lead to unconnected nets, which you might not notice while drawing.

    You can check if a net connects to a pin by using the "show" symbol represented by an eye on the top left of the screen. If the pin is highlighted there is a physical connection between net and pin. If the pin doesn't highlight you can be sure there is no connection.

    The ERC (Electrical Rule Check) will not show you unconnected nets. It will put out error messages about unconnected input pins only!

    You might use the equivalent values for several grid sizes like 1.27, 0.635, 0.3175. 0.15875 or even 0.079375mm and still get the nets connected, getting critical with smaller grids. You might to the same within the board editor.

    If you save your work with a metric grid it should reload with the same grid setting.

    Finally I recommend not to mess with the SCR files unless you know exactly what you are doing.

    Regards

    Boncuk
     
  4. dave

    Dave New Member

    Joined:
    Jan 12, 1997
    Messages:
    -
    Likes:
    0


     
  5. Angry Badger

    Angry Badger Member

    Joined:
    Jun 29, 2008
    Messages:
    201
    Likes:
    8
    Location:
    Flintshire, North Wales

    Hi,

    Thanks Sceadwin,

    I want to set mm as the default units, only using Imperial when I select that manually, i.e. don't want to have to set mm every time I open up the file. I hadn't seen that pdf before, it looks to have lots of useful info in it so I will read it later. Thanks.

    Thanks Boncuk,

    Is it really neccessary to use Imperial? Datasheets for many of the most recent components have metric units as their primary dimension units, certaintly for some of the passives for which I've been making library components. If I design all my own library components (tedious sometimes though it is) using metric units and layout both the schematic and pcb on a metric grid, should that be a problem?

    I know what you mean about off-grid and angle errors as I'm getting a lot of these on my current pcb because I've used both metric and imperial. It's a bit of a mess in that regard but as it's a home made pcb I'm not too worried so long as it looks neat.

    Stepper_pcb.png
     
  6. Boncuk

    Boncuk New Member

    Joined:
    Nov 10, 2007
    Messages:
    5,382
    Likes:
    88
    Location:
    Phetchabun,Thailand
    Hi Angry Badger,

    most boards containing SMD components still contain inch-based ones like caps, tactile switches and connectors.

    SMD parts are manufactured in a metric scale, but there also some amongst them with a pin distance of 0.35mm. Using a grid size of 0.3175 the grid is still inch based (25.4/80=0.3175) and will give you the necessary resolution. If that won't suffice use 0.15875mm or even 0.079375mm. I sometimes use a grid size of 0.0396875mm if circumstances require to do so.

    Using that grid and draw traces out of the SMD pad the joint will be straight in.

    I noticed on your board design that all (probably pushbuttons) have air wires within all four SMD-pads caused by grid mismatches which can be eliminated if you use the above described method for routing. (Don't forget to blank layer 19 ("unrouted") when printing the PCB layout.

    You will see that when performing "ratsnest". The autorouter will point out all air wires without creating an error list.

    A neat PCB layout is neat if there are no acute angles in traces. Your design is full of those acute angles making etching more difficult. If traces join at a 90 degree angle draw two 45 degree angled off traces manually to meet on the trace they angle off. (Please refer to the attachment.)

    I have done a lot of PCB designs with mixed through hole and SMD parts and using an inch based grid I had absolutely no problems. The autorouter will not work properly if you use a metric grid because it also uses inches or fractions thereof.

    Regards

    Boncuk
     

    Attached Files:

Share This Page