Trace cleanup / rounded ends. (Urgent!)

[dogboy]

Hi,

I am trying to connect a few high powered leds in series, but would like to use a 1mm minimum trace width.

However, in this case, if I use a width above 0.6mm the rounded ends of the track extend the other side of the pad.

How can I clean up the tracks to remove this?
I have looked, but cannot find an answer to this.

Attached is a screen shot showing in detail what I mean.

Any help would be appriciated.

Thanks

[Tomg]

I don't think trace-end trimming is possible in DipTrace. Could be wrong, of course. To solve your problem in DipTrace, first make sure the two pads belong to the same Net. If you are not working with a schematic, connect them to each other using the Place Ratline tool. Once they belong to the same Net, draw a copper pour of the size and shape you need between them (~pad center to ~pad center). Finally, connect the copper pour to the same Net. Make sure to select "Direct" in the copper pour's Thermals drop-down list under the [Connectivity] tab. Also, uncheck (disable) the "[ ]Separate Thermals for SMD" option.

[dogboy]

Hi Tom,

Thank you for your reply, its appreciated.

Yes that would work and I did try this, but the board I want has hundreds of these footprints, which all need connecting, which is very time consuming.
I really would like to just add a track as normal. Will also allow me to edit the board easily if required.

I was hoping for a quicker solution.

What I am now trying to do is extend the size of the two outside pads, which allows me to connect a wider track.
But as I need the same size actual pad for the SMT part, I have edited the library with a top mask over the part of the pad I don't want exposed. (Bigger pad, with a mask on top, leaving the size of the original pad exposed)

So, in this case the pad is 0.6mm x 3mm (Actual what I need as a exposed pad)

After editing the pattern the pad is 2.6 x 3mm but with a 2mm x 3mm top mask area, which leaves the original size (0.6 x 3mm) and the rest of the pad will be covered with the solder resist.
I am assuming that the top mask is a solder resist mask?

Seems ok, but need to test it. (Not sure how to confirm of check this yet?), not sure if this will work.
Works when connecting the tracks and doing the layout, but when the board is made will the only the original pad sizes be exposed??

Thanks for your input.

Paul

[Tomg]

"...I am assuming that the top mask is a solder resist mask?..."

Hi Paul,
Unfortunately, any filled objects drawn on the Top Mask layer will make custom openings in the solder mask. This can be confirmed by using the 3D Preview tool in the PCB Layout editor. You should also be aware that these custom openings are not affected by the Solder Mask Swell setting found in the Gerber Export tool.

Another thing you might want to try would be to see if the automatic neck-down would get you close to the desired result. The wide part of the trace might stand off a little from the pad, but you could go to a smaller grid size and drag the wide segment closer to the pad to contact it as much as possible without hanging it over the back side. That might speed things up a little, then you could come back later and copy/paste in some small copper pours to cover any gaps that might remain.

For an example, see the video inside the attached zip folder named "routing.zip" below...

[dtu2]

Hey Paul,

There is one other thing that may work for you. You can run multiple traces between the pads and them move them together to simulate one larger trace. I've included a pic to demonstrate.

The R1/R2 example shows the multiple traces separated from each other.
The R3/R4 example shows the three traces moved adjacent to each other to simulate one wider trace.

However, it could be a lot of work if you have 'hundreds' of them.

Jeff

[dogboy]

Hi Jeff,

Thank you to everyone who has replied.

I tried my suggestion (Extend the pads in the footprint), which worked fine from a track point of view, but the resist mask was not correct.
Even though I placed a resist area of the unexposed part of the pad in the footprint.
Shame really, because that would have been a nice easy solution.

Anyway, after looking at everyones suggestions, I will play around with each and see what is going to be the quickest and most suited for editing later.
I think the multiple tracks moved together is more than likely what I will use.

Thanks again.

Cheers

Paul

[Jason Bonner]

Not sure if this suggestion fixes your issue, but I've laid out a couple boards with 3.5mm LED pads, and ran into the same issue as you did. Here's what I did to fix it:

In this particular case I wanted 40mil trace between the two pads, but it would stick out either side of the narrow LED pad, so I started with something that wouldn't, in this case it was a 20mil trace. Then I bumped it up to a 40mil, and then back down to a 20mil, as seen in the 1st screenshot.

2nd screen shot I dragged the 40mil trace to the very edge of the LED pad.

3rd screen shot is what the final trace looks like.

[bpjl]

so I started with something that wouldn't, in this case it was a 20mil trace. Then I bumped it up to a 40mil, and then back down to a 20mil

dragged the 40mil trace to the very edge of the LED pad.

Man, you are a genius