0
\$\begingroup\$

I've done rigid-flex PCB designs a number of times in the past but it was long enough ago that I cannot remember how I solved this issue. My design has three sections - the main board, the flex, and a daughter board. The flex obviously connects the two rigid boards. The problem is that I cannot seem to place tracks across where the split lines are defined, meaning using the interactive routing tool I can't run traces from the main board over the flex to the daughter board. When I place a trace and move it so that it crosses the line, the error I see is this:

enter image description here

Altium clearly thinks that just because I go from a rigid section to a flex section, that I am going outside the board outline (which is not true). I have no idea what the poly region is, and I do not see anything on the "Multilayer" layer indicating a poly region.

My board stackup is shown below:

enter image description here

I have tried running tracks on all of the four layers and all of them behave the same way.

How does one draw tracks across different sections of a rigid-flex design? My guess is the problem has something to do with the stackup but I can't place my finger on it.

I am using Altium Designer 18.1.7.

\$\endgroup\$
2
  • \$\begingroup\$ I have a gut feeling, though no certainty (not at Altium PC right now), that this is due to the fact that your non-conductive layers change material between sections in the bottom view. If that is the case, that may be fixable without changing that "discontinuity", though I'd have to try a few things to figure it out myself, but first experiment, force them continuous and see what happens. Clarity: I think it sees no way of attaching your daughterboard to the whole, due to the stackup incompatibility and just gives up. \$\endgroup\$
    – Asmyldof
    Commented Jun 27, 2018 at 18:11
  • \$\begingroup\$ I'll be talking to my manufacturer about this. I was able to get around the error simply by turning off the "board outline" constraints in the rules. A "split line" is defined as a "board outline" and prevents me from routing straight through. That being said, the stackup is still something that needs exploration and I'll need to communicate with our vendor for that. \$\endgroup\$
    – DerStrom8
    Commented Jun 27, 2018 at 18:30

2 Answers 2

Reset to default
1
\$\begingroup\$

Using Altium Designer 19.0.15, there is the option to change the clearance for "Split Barriers" which allows you to keep the standard board outline clearance and still rout on rigid-flex boards. In the picture below, the highlighted cell allows you to cross flex-to-rigid boundaries when set to zero.

Board outline clearance rule page

\$\endgroup\$
0
\$\begingroup\$

It looks like your layers are not continuous between your stackups. The copper layers in a rigid flex are usually sandwiched on the inner layers, like this:

enter image description here

But maybe your manufacturer uses a different stackup.

I would make your stakup look like this ( the inner layers are continuous) and make sure you put the flex overlays on the flex section and see what happens.

\$\endgroup\$
2
  • \$\begingroup\$ The problem with that is that I don't want a 59 mil core through the middle of my flex. I did check another tutorial and they used two of the upper layers instead of the two center layers \$\endgroup\$
    – DerStrom8
    Commented Jun 26, 2018 at 19:57
  • \$\begingroup\$ Actually, it's one of the examples that came with Altium: youtube.com/watch?v=aeRd1b6oGto \$\endgroup\$
    – DerStrom8
    Commented Jun 26, 2018 at 20:09

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.