[PCB_FORUM] Re: Moving to V16.01 -- any issuses?

Hi Sue
 
Just a couple of comments about below:
 
From memory, it may report it cannot find library parts when it's actually having trouble trying to create components with older padstacks, ie pre-v15.  That may be a clue.
 
Constraints haven't gone.  Well, NET_SPACING_TYPE and NET_PHYSICAL_TYPE have been removed but the values have been transferred to other areas in the constraints that make more sense.  We now no longer have a total kludge of "old" constraint setups and "new" constraints in the Constraint Manager.  I agree - it definitely takes a day or two to get used to it but in my opinion it's better and cleaner.  Multi-layer diff pairs are pretty good.
 
We don't use OpenGL because highlighted traces do not have the good old 'dotted line'.  They look like another layer, unless you zoom out - then the dotted line appears it's but next to useless because you've zoomed out too far.  According to our Cadence AE, this is a feature of OpenGL.
 
We used to see a lot of SAV files in the earlier releases of 16.01.  Not so many now, just the 'usual' (ie not often at all.)
 
Hope this helps.
 
Cheers,
Richard
 
 

__________________________
Richard Moffat
PCB Specialist Engineer
Allied Telesis Labs
ph. +64 (3) 3393000
richard.moffat@xxxxxxxxxxxxxxxxxxx


>>> On 20/08/2008 at 12:30 a.m., in message <58292FA6B3EEFD49AEDAF6597E21E7170A70C7AE@xxxxxxxxxxxxxxxxxx>, "Reade, Sue" <Sue.Reade@xxxxxxxxxxx> wrote:
I ran into problems with memory write errors - I ended up having to turn off open GL, this did not completely solve the problem but it reduced it to about once per day. going back to v15 ended the memory write errors completely.
I ran into problems bringing in library symbols, all of our symbols were either created in 14.2 or 15.5.1. the 15.5.1 symbols came in just fine, but the 14.2 symbols brought up an error of symbols too old must be uprev'd. I upreved the library, which created it's own set of issues but it did not completely solve the problem. My best guess was that there was another issue associated with the netlist and symbols but that this was the error continually being pulled out of the bit bucket.
The pass over feature, where the tool tells you what you are going over needs some work.
Moving in and out of working with placement features and then moving into wiring features also needs some work, it would get stuck in one mode or the other and it took some messing around to get it to obey commands.
.SAV files being created from the .BRD files constantly - no reason found for this as the .BRD did not appear corrupted, or at least when DBdoctor was run no errors were reported and the original file could be saved out successfully sometimes as a .BRD.
The final straw for me was when it inexplicably could not longer update models from the library because it could not find the library, even though the path when checked with SET on the command line was absolutely correct.
I'm just going to wait until they come out with a higher rev and try again.
If you go to 16.01 besure that you have time to check it out thoroughly before you start a working design. Definitely give yourself about 3 days of playing with it to find where the commands have been hidden. Cadence did not fix anything with the GUI, most things are just in a different location. The constraints are gone, and you will be completely at the mercy of the constraint manager. This can be good or bad depending on your experiences with that part of the tool.
It does have some improved features. the manual wiring options are much improved. It does take a v15 .BRD forward well and transfers all of the information stored in constraints to the constraint manager accurately. However it did not take a 14.2 .BRD forward well at all, even when that board was uprev'd to v15 and then moved forward. the graphics might be better but with the memory crashes, I could say that it was worth it. I did not get far enough with it to try the router interface, but it does look a bit more streamlined.
Good Luck.
 

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Sawyer Jayne
Sent: Monday, August 18, 2008 7:01 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Moving to V16.01 -- any issuses?

I sent this post last week but got very little response so I thought I would try again under a new subject …

 

 

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Sawyer Jayne
Sent: Thursday, August 14, 2008 7:23 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Changing NPTH hole size on one instance of a symbol...

 

We are planning to move to V16.01 soon so I am curious about Sue’s reference below to issues with the new software. Sue can you describe specifics? Are others still holding off on going to version 16.01 due to stability or other issues?

 

 

Jayne Sawyer

Engineering Tools Support  

 

-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Reade, Sue
Sent: Wednesday, August 13, 2008 1:40 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Changing NPTH hole size on one instance of a symbol...

 

What version of allegro are you using?

In V15.x

Tools

Padstack

Replace

Select the pin - it should immediately pop up in OLD

Select ... On the NEW line

Select your new padstack

Enter Symbol, pin# or Refdes fields as needed

Replace

Done

Wait for DRC to run.

Now if it is a  mechanical symbol, you may have to go back to the

libarary and modify the model and refresh it.

 

If you are in 16.01, I ran into this problem big time among other

things, and decided that 16.01 is too fragil for production work.

 

 

-----Original Message-----

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx

[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Austin Franklin

Sent: Wednesday, August 13, 2008 4:32 PM

To: icu-pcb-forum@xxxxxxxxxxxxx

Subject: [PCB_FORUM] Changing NPTH hole size on one instance of a

symbol...

 

Hi,

 

How do I change the NPTH hole size on only one instance of a symbol I

have on my board?  I swear I've done this easily many times in the past,

but just can't remember how I did it.  I've of course tried editing the

padstack in instance mode, and did the edit...but the new padstack name

doesn't seem to take effect...it still has the old padstack name and

info.

 

Regards,

 

Austin

 

-----------------------------------------------------------

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

-----------------------------------------------------------

-----------------------------------------------------------

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: