[PCB_FORUM] Re: Impedance controlled line widths

Dave,

With all respect, few fab shops measure, or indeed are able to measure, 
impedance at 1GHz+. Most use tools like Polar CITS or
similar. With tr/tf in the order of 50ps to 500ps most of their means of 
verification are becoming increasingly irrelevant.

Where it matters I specify materials sometimes down to vendor PN's, including 
masks, and take into account etch and lamination
processing.


Best Regards
 
David Greig
______________________________
GigaDyne Ltd
5 Albany Business Centre
Gardeners Street
Dunfermline KY12 0RN
United Kingdom
t: +44 (0)1383 624 975
www.gigadyne.co.uk
______________________________

-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dave Schaefer
Sent: 29 August 2007 16:17
To: icu-pcb-forum@xxxxxxxxxxxxx; icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Impedance controlled line widths

Jean / David,

I always consult with my fab shop, as their processes impact the impedances 
yielded. I have had many designs which have required
material / feature adjustment when transitioning from prototype fabricator to 
volume fabricator.

Here's my basic process:
- evaluate my impedance requirements using available calculators / cad tools, 
factor in any other requirements to come up with a
desired stackup.
- send the critical design details to the fabricator for comment & 
recommendation (stackup, materials, trace widths &
clearances, etc.).
- modify my design to satisfy design intent and fabricator capabilities.

There's no CAD tool or calculator that contains "process effective dielectric" 
constants for every PCB vendor.

Hth,
Dave

> 
> From: "David Greig" <david@xxxxxxxxxxxxxx>
> Date: 2007/08/29 Wed AM 09:54:06 CDT
> To: <icu-pcb-forum@xxxxxxxxxxxxx>
> Subject: [PCB_FORUM] Re: Impedance controlled line widths
> 
> Hope this is what you mean: the impedance property is overruling the physical 
> type.
>  
> Set environment variable acon_no_impedance_width in the etch category.
>  
> Off topic, but is anyone else getting fabs telling you that your track 
> widths for microstrips are off because they are calculating using the 
> latest Polar tool? I use a couple of BEM, MOM and several different 3D full 
> wave tools that are in closer agreement to each
other than the values the fab shops are reporting back.
>  
> Best Regards
>  
> David Greig
> ______________________________
>  
> GigaDyne Ltd
> 5 Albany Business Centre
> Gardeners Street
> Dunfermline KY12 0RN
> United Kingdom
> t: +44 (0)1383 624 975
> www.gigadyne.co.uk
> ______________________________
>  
> 
>   _____
> 
> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Jean Bratton
> Sent: 29 August 2007 15:10
> To: icu-pcb-forum@xxxxxxxxxxxxx
> Subject: [PCB_FORUM] Impedance controlled line widths
> 
> 
> 
> Hi folks,
> 
> We have a design with impedance rules built in at the schematic level. 
> The stackup appears to be correctly defined as provided to us, but 
> Allegro is not calculating the trace widths at the same width as the 
> stackup indicates they should be. The impedance value appears to be 
> the prevailing rule, not the trace width we have set up in the 
> constraints. If we delete the impedance property, we can get the board to 
> route with the trace widths we specify, but we're
wondering if there's a way to change the priority.to have it look at what the 
design rules specify for trace width rather than
what the impedance rule would automatically define.
> 
>  
> 
> Also, does anyone know of a good impedance calculator online? The one 
> we used to use isn't set up for a board as thick as this one is, so we 
> need another. We need to know which is accurate, the stackup provided to us, 
> or the calculations Allegro is making.
> 
> Thanks for any insight,
> 
> Jean
> 
>  
> 
> Jean Bratton
> 
> Sr. Printed Circuit Designer
> 
> Freedom CAD Services, Inc.
> 
> 603-864-1349
> 
>  <mailto:jean.bratton@xxxxxxxxxxxxxx> jean.bratton@xxxxxxxxxxxxxx
> 
> Visit us at  <http://www.freedomcad.com> http://www.freedomcad.com
> 
>  
> 
> 
> This correspondence and any attachments are considered confidential. 
> If you are not the intended recipient, please notify Freedom CAD 
> Services, Inc. immediately by either replying to this message or by sending 
> an email to operations@xxxxxxxxxxxxxx; please
destroy all copies of this message and any attachments. Thank you.
> 
> --
> 
> Virus scanned by Lumison.
> 
> 
> 

Dave Schaefer
dave.schaefer@xxxxxxx
-----------------------------------------------------------
To subscribe/unsubscribe: 
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe

To view the archives of this list go to 
http://www.freelists.org/archives/icu-pcb-forum/

Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
--
Virus scanned by Lumison.

-----------------------------------------------------------
To subscribe/unsubscribe: 
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe

To view the archives of this list go to 
http://www.freelists.org/archives/icu-pcb-forum/

Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------

Other related posts: