Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

microstrip layout, print tolerances

Status
Not open for further replies.
B

bejing

Member level 2
Member level 2
Joined
Sep 7, 2015
Messages
42
Helped
0
Reputation
0
Reaction score
0
Trophy points
6
Activity points
330
hi
when we design a rf layout for example in ADS, and then send it to a PCB Manufacturer,
they print the layout on a laminate.
in the photo-etching process, several undesirable effect will occur on pcb trace width.
can anyone explain what type of effects can occur. and how we can compensate for that errors (pcb fabrication errors)?
is offseting the boundry of trace, an issue?

thanks.
 

Nothing you can compensate for. Expect the copper structures to be reproduced typically with designed size, but variations of +/- 50 µm trace width can occur in usual high density process (100 µm minimal width/spacing), more in lower quality process.

Also considerably variations in substrate height and permittivity must be considered, refer to substrate manufacturer specifications.

If these variations can't be accepted, order impedance controlled manufacturing. Contact your PCB manufacturer for details.
 
  • Like
Reactions: bejing

    B

    bejing

    Points: 2
    Helpful Answer Positive Rating
thanks sir FvM,

in ADS CookBook (v2):
Process Variations and Discrete component tolerance:
There are multiple sources of variations in the real microwave world which could be associated with
Dielectrics, Etching Process and Discrete components etc.
a. Dielectrics: Dielectrics can have variations in their height, loss tangent and dielectric
constant (Er) and this data can be obtained directly from manufacturer’s datasheet.
b. Etching: Etching tolerance in printed circuit process is dependent upon the etching
technique used and this tolerance mainly affects the width of the transmission lines.
i. Chemical etching process can have tolerance level of +/- Metal Conductor Thickness
(max.).
ii. Reactive ion etching can produce the excellent tolerance of +/-1um.
iii. Metal deposition techniques could also produce tolerance of +/- 1-2um
c. Discrete components: Discrete components like Inductors, Capacitors, and Resistors etc
have their inherent tolerances which could affect circuit performance. Different
tolerances for discrete components are summarized in Table 1.
Click to expand...

in part b, it seems to said that we may offset thickness/2 the trace width for compensating the error.
 

I have seen a PPT presentation where Monte-Carlo simulation was used to evaluate tolerances impact on the design and choose better values for capacitors and resistors. I think it was ADS, but i googled for it and did not found it. Maybe the same method could be applied to microstrip element width/spacing.
 
  • Like
Reactions: bejing

    B

    bejing

    Points: 2
    Helpful Answer Positive Rating
thanks dear Terminator3.
i did testing my first edition of pcb that the length of p-p was about as large as 20 lambda.
for such a complicated circuit it was hard to predict the effects of fab errors.
but now, i know the errors due to test results.
i wish to find some tips for compensating the fab-errors. although dear FvM said that no need to compensation.
another error may be curving inner corner of 90deg bends in the etching process.

- - - Updated - - -

i am using rogers duroid laminate, I thought rogers have the best reliable laminates... i must recheck datasheet.
 

i did testing my first edition of pcb that the length of p-p was about as large as 20 lambda.
for such a complicated circuit it was hard to predict the effects of fab errors.
but now, i know the errors due to test results.
Click to expand...
If you have already a prototype, what are the actually observed dimension errors?

Problem is however, that a new batch must not necessarily achieve exactly the same size variation as the prototype, unless the manufacturer can assure you to keep everything constant. Most likely he can't. That's particularly the case for prototype production in pool service.

That's why impedance control is the preferred method to reproduce RF/high speed PCB exactly.

Some typical parameters of the PCB manufacturing process can be of course reflected in your design simulation like the trapezoidal trace shape and the said corner rounding.
 

    V

    Points: 2
    Helpful Answer Positive Rating
It's a question how much the Transmission Line (or any line ) is critical ?? For instance a TL that is used simply match an impedance at 500 MHz is much less critical compare to another one that works for a VCO @ 60GHz..
So it depends on the specific application.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top