• 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.

EAGLE software question, trace sizes

Status
Not open for further replies.

mramos1

Active Member
I am no expert on Eagle CAD but it works great for me. But the default
traces are too thin and I sometimes leave the boards in too long (I use the copy paper method and it works great, I just get busy, and forget for an extra 5 minutes to remove the boards). I then use a metal ink pin (circuit write) and fix it. Looks like poo..

Does anyone know how to change the track thickness? Can I do a board that is complete, or have to set it before I do the board?
 

4electros

New Member
I think you have to set the board before you do it , go to :
Tools,DRC... then choice <<sizes...minimum width, minimum drill
there are also many options regarding board layout but that's the basics you might need.Then if you want to save those settings go to : DRC<<FILE<<SAVE AS ....
i hope that i could help more!
 

Oznog

Active Member
All trace sizes, actually everything, should be set on the schematic.
Every trace has a Net Class associated with it. If you haven't been specifying it, they're all part of the Default class which has no width specified, so width defaults to 10mils during the Routing stage.

So, go under Edit->Net Classes, Default-Width-30 mils (or whatever floats your boat).
You can also add say a Power class and make it thicker. You can specify this when making connections. Or you can Edit->Change->Net Classes, select Power, double click on each wire you want to become part of the Power class. This is how you can have thick and thin wires coexisting on the same design.

It is also possible to route the board and change with width of individual trace segments. Generally this is not the right way to do it and it will raise warnings on your Design Rule Check but it's otherwise ok. Sometimes you have to do this to make a thick power trace used for Vdd or Gnd turn into a thin trace over a short trace stub in order to connect to a fine pitch SMD pad without extending over the neighboring pads.
 

DirtyLude

Well-Known Member
To do it the 'incorrect way'. There's a 'change' icon on the toolbar (looks like a wrench). If you select it, it will give you a list of things you can change. Select width, then the trace width you want to change to. Then just start clicking on the traces you want to enlarge. The traces will change to the width you specified.
 

philba

New Member
or, use group to select all your traces, use change/width, then right click on anything in the "selected group" and all traces in the group will be set to the selected width. If you display only top and bottom layers before doing that, you can avoid changing other lines (like on the silkscreen or what ever).

in general, group is a very powerfull tool to use in conjunction with other tools. For example, you can rip-up an area of the board via this. or you can "smash" all your components at once. and so on.
 

Oznog

Active Member
DirtyLude said:
To do it the 'incorrect way'.
Um yeaaah... that's the wrong way to do it (yet somehow you still want to bring it up?). You put the board out of sync with the schematic for no reason at all, and it basically can't be undone so it will curse your design forever. Don't do it. This is only appropriate if you want to make some branches of a net a different width than others (like the aforementioned SMD case) or you don't have the schematic (in the odd scenario that you are given a board with no schem).
 

philba

New Member
I don't think there is anything wrong with it. I do it all the time and never get out of sync. maybe you are closing the schematic and modifying the BRD? that's a way bad idea as it does cause sync problems.

DRC will only complain if you make the trace narrower than the default for the class. which kind of makes sense. for example, I use 20 mil default for power but for HBridges, I beef up the power trace to something appropriately wide - like 50 mil. it's a power trace but needs more current. DRC is happy as a clam. yeah, I could create a special class but for a couple of traces, it's not worth it.
 

mramos1

Active Member
Oznog, Thanks.. That is the right way for my future projects.

Lude and Philba, that will solve a couple old boards already done.

Thanks guys, and thanks Oznog as I would be asking about the power traces probably later if I did not see it in that list :)
 

DirtyLude

Well-Known Member
Oznog said:
Um yeaaah... that's the wrong way to do it (yet somehow you still want to bring it up?).
So there's reasons for it, but you don't want anyone to know how. That makes no sence.
 

mramos1

Active Member
Yep, there is. This thread solved three of my problems, one I had not ran into yet.

I found the wrench before I posted, and selected the traces and did not see them get thicker. I will try again night. I will group, click the new size and print it, maybe it is not visible on the screen.

But thats again guys. I think this will be a good search items for the forum.
 

DirtyLude

Well-Known Member
When you select the wrench, you then have to select width from the drop down, then the track width you want. If you select Size or Spacing or anything like that, it wont work.
 
Status
Not open for further replies.

Latest threads

EE World Online Articles

Loading
Top