BEWARE - FLIPPED FOOTPRINTS!

[mtripoli]

Hello,

I got a call from a client this morning that one of the boards I had done for him had a few footprints "flipped" (we both use DT).

My response was "That is impossible". Upon opening the file, the footprint for a 28 pin PIC was in fact "flipped" as were a couple of diodes.

Now... I did NOT "flip" any component footprint. In fact, I will go so far as to say, in 39 years of laying out PCB's, I can not come up with a single, legitimate reason to flip a footprint. I go by a very simply philosophy; if it can't be done in the "real" world, it should NOT be done in the software. I use this same mandate when designing in Solidworks, and I have never had a model "break" or a tool maker tell me one of my parts couldn't be tooled.

What is totally perplexing about this whole situation is, as I've already said, I did NOTHING that should have flipped the footprints. What I did do is take a design that had already been worked on, open it on my system, CHANGE SIDE of a bunch of components, then re-routed the board. I use real-time DRC, at no time did I ever get a message that anything was "flipped" (though as pointed out, when one hovers over the FP, it does say "flipped"). How could this have happened? It seems to me that one has to go out of their way to do this, yet it happened.

In this case, thankfully, only 10 proto boards were made, and one populated. Not a lot of stuff on the board, but this COULD HAVE been an absolute, unmitigated disaster.

I'm not being facetious, or antagonistic; could someone with experience please tell me in what situation one would want to "flip" a footprint vertically or horizontally?

I, for one, will please ask, NO, BEG THE DEVELOPERS to take out this feature.

Mike Tripoli

[Tomg]

Actually, the Group Flip tool in the PCB Layout editor should be retained, but changed so that any footprint within that selected group is not flipped during the operation; just flip its position in relation to the other objects being flipped. This can be a very powerful and useful tool as long as its ability to flip the pattern itself is removed from the algorithm. Am I making any sense here or did I just confuse the issue?

p.s. See my related post labeled as "#17" (Tomg) on this page - viewtopic.php?f=20&t=11893&p=23424

p.p.s. If a component's pattern somehow ends up flipped, the Design Rule Check should be modified to find and flag the offender.

[mtripoli]

On the money, TomG... Being able to "flip" stuff, like polygons, etc. is great. "Flipping" footprints is very, very bad... It should change a different color, OR SOMETHING, or just not flip at all...

Mike Tripoli

[mtripoli]

Hi,

I'm not trying to be an alarmist, and I AM NOT trashing Diptrace, BUT IT HAS HAPPENED AGAIN!

This time, I took an existing design that had a linear supply on it, did ALL NEW SCHEMATIC UPDATES for a switcher and updated the PCB. I got a call; the switcher IC is flipped.

PLEASE, HOW CAN THIS HAPPEN? These last few were small, less than 50 component boards. However, I'm about to begin laying out a new audio amplifier; am I going to have to continually check footprints to see if they're "flipped"? If so, this is no longer a tool but a liability.

PLEASE PUT OUT A PATCH THAT DOESN'T ALLOW FLIPPED FOOTPRINTS! I posed the question before; why? Why would anyone ever want to flip a footprint...

MT

[novarm44]

The feature which allows to flip footprints has been changed for the next update: only position of footprint will be flipped with the group + warning shown. Plus we will also add check and warning before exporting Gerbers/ODB++ for existing layouts.

Please always use compare to schematic - it reports flipped footprints.

[mtripoli]

So, to clarify, it will not be possible at all to "flip" a footprint under any circumstances? Or it can still be flipped with warnings?

Please explain: What does "Compare to Schematic" do that "Check net connectivity" does not? What is in the schematic, other than the net list, that should need to be checked against the schematic? Having the ability to "Compare to Schematic" does indeed show the flipped components (which in this case, as it turns out, there were eight (8) flipped footprints! Thankfully they're all resistors and caps).

How is this happening in the first place? I did nothing to flip anything, and to "unflip" them is nothing less than three (3) mouse clicks per footprint. So, unless there is some magic combination of keys that I'm hitting, or there's an undocumented hotkey, I cannot begin to understand this...

I definitely have a "love/hate" relationship with DipTrace. On one hand, it's relatively easy to use, and having 3D step export is great. But when stuff like this (flipping footprints out of nowhere) starts to happen, it is no longer a tool... I have recommended Diptrace to many people, most of whom have tried it, and a few bought it. When this kind of stuff happens, it makes it hard to tell someone "try it, but..."

MT

[novarm44]

It will not be possible at all (already done). The feature, which can do footprint flip is called "Edit / Flip Group" and it was there since first versions, there is no hotkey by default, but it is possible to aasign it.

Net connectivity check finds if all copper connections are identical to net-list (no shorts and breaks).
Compare to schematic compares PCB netlist to Schematic netlist, also footprints if they are identical to specified in schematic, and a few other things that should be identical in PCB and Schematic.

[mtripoli]

Okay, thank you for the explanation.

I'm glad to hear the 'flip' prevention is already done. Is this available now for download?

Thanks again,

Mike Tripoli

[novarm44]

It is not available yet. Will appear in the next update.
With current version just avoid using Edit/Flip Group feature with components and
always use Compare to Schematic before exporting gerbers (even with next versions, not because of this issue only).

[grimepoch]

I cannot believe you guys took out this feature for people that actually DO use flip footprint, instead of just addressing the bug that you had that wasn't doing the right thing.

When I insert board connectors, it is much easier to have the pin numbering be identical between 2 boards and the just flip the pattern on the receiving end of the board so that things line up. I verify all the pins visually with both boards up.

With this change you have forced on us, I now have to rewire a very large connector in reverse direction it seems. (Although it appears older boards will remain flipped, it just won't let you flip new things)

I get that this is very bad for component footprints of the nature of IC or anything with more than 2 pins that are not symmetrical, but there are cases where it makes sense. It seems the upgrade I just paid for was a downgrade.