Bryan,

First,  to change Routing mode while in the interactive router press SHIFT+R
this will cycle through the 3 modes.  To see which mode you are in glance at
the command or status bar(can't remember which)

Avoid(follows clearance rules to disallow short circuits) - This is the mode
it has been routing in... and why you cannot reach that pad.
Ignore obstacle(Will allow you to route anywhere and break your clearance
rules at will)
Push Obstacle(Will attempt to 'push' tracks that would cause a clearance
violation to keep them within the specified clearances)

The major factor in the Avoid Obstacle mode is that in order to connect two
objects they must be of the same net.
Two objects marked as NoNet will be considered of different nets.

The thing to consider with using the Ignore is that there is a reason it is
stopping you while in Avoid mode, and ignoring that will lead to a violation
which you will need to eliminate eventually anyway.

So... the first thing to look at is to make sure that both objects have the
same net, or any net at all.

If both objects have the same net, we need to look at some other
things(hopefully one will lead to a solution)

BTW as an aside..  I would be happy to look this file over for you if you
want to zip it and e-mail it to me.  I will find the problem and let you
know what it was.

Ah... I just noticed something.

>> I remember asking this question once and was told to "Clear Nets",
>>"Update free primitives", then to reload my netlist.

If you went through this in the steps listed above, in that order, you will
have a board full of NoNet violations.  The pads would have nets... but not
the tracks.

This procedure is out of step... maybe this will help.  Try this order
instead.
Clear Nets
Load Nets
Update Primitives <-- this process requires that component pads have netlist
information.

Another thing I would check for would be duplicate net names(I am unsure
what causes these... but I have seen them)

Go to Design-->Netlist manager

Highlight the netclass for ALL Nets... and then browse through the list
looking for double entries.

Well... I am starting to get into the obscurities here..  ;)

Let me know if any of this helps, if not we will check some of the more
obscure things that could cause this.

----------------------------------------------------------------------
Colby Siemer                        ** Custom Battery Chargers
                                           ** Custom Power Supplies
PowerStream Technology       ** Custom UPS
140 S. Mountainway Drive      ** Custom DC/DC Converters
Orem Utah 84058                  ** Power management electronics for OEMs

http://www.PowerStream.com

----- Original Message -----
From: Bryan Bernesi <[EMAIL PROTECTED]>
To: Multiple recipients of list proteledausers
<[EMAIL PROTECTED]>
Sent: Tuesday, February 27, 2001 8:46 AM
Subject: Re: [PROTEL EDA USERS]: reconnecting nets


> Hello Tom, Colby,
>
> Tom, yes I'm sure they connect. The autorouter routed the connection for
me,
> but routed it with changing layers and adding vias where there is no need.
> What I wanted to do is remove the via and changed layer and to reconnect
the
> 2 pads with a single straight trace.
>
> here are some more details,
>
> Pad A (10400, 11950) - [NetU2_TG_8] - Pin 5 of a 5 pin sip
> Pad B (10500, 11950) - [NetU2_TG_8] - Pin 4 of an 8 pin DIPSWITCH
>
> I checked to see if there was anything underneath the pad, and there was
> nothing.
>
> Colby, you are on the right line of thinking  though....... my whole board
> lights up like a christmas tree with clearance violations, even though
there
> shouldn't  be any. I have someone at the Protel Tech support looking into
> this for me. I remember asking this question once and was told to "Clear
> Nets", "Update free primitives", then to reload my netlist. It didn't
work.
>
> How do I set the interactive routing to "Avoid Obstacle"?
>
>
> Very kind Regards,
>
> Bryan Bernesi
>
>
> ----- Original Message -----
> From: "Tom E Luttrell" <[EMAIL PROTECTED]>
> To: "Multiple recipients of list proteledausers"
> <[EMAIL PROTECTED]>
> Sent: Monday, February 26, 2001 5:14 PM
> Subject: RE: [PROTEL EDA USERS]: reconnecting nets
>
>
> > The brute force way to do this may be to change the Preference for
> > interactive routing to 'Ignore obstacle'. Then after placing the track
> > between the pads (are you sure they connect??? Check both their nets
> first)
> > select the track and change the net to the same as the connected pads.
> Don't
> > forget to change the Preference for interactive routing back to 'Avoid
> > obstacle'
> > I have not had this problem before, do you have service pack 6
installed?
> >
> > Tom L.
> >
> > -----Original Message-----
> > From: Bryan Bernesi [mailto:[EMAIL PROTECTED]]
> > Sent: Tuesday, 27 February 2001 2:47 AM
> > To: Multiple recipients of list proteledausers
> > Subject: [PROTEL EDA USERS]: reconnecting nets
> >
> >
> > Hello,
> >
> > I have finally got my board routed. Now, I am still having problems with
> the
> > nets.
> >
> > The autorouter routed a net stupidly (it put a via, and changed layers,
> > where there is no need. The connection is in-between 2 pads 100mil
apart).
> > So I deleted the trace and the via and tried to reconnect it, but protel
> > will not allow me. I think it comes up as a DRC.
> >
> > I remember asking a question like this before and I was told to clear
nets
> > and reload them. I did try this, without success.
> >
> > any ideas?
> >
> > Bryan Bernesi
> >
> > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
> > *  This message sent by: PROTEL EDA USERS MAILING LIST
> > *
> > *  Use the "reply" command in your email program to
> > *  respond to this message.
> > *
> > *  To unsubscribe from this mailing list use the form at
> > *  the Association web site. You will need to give the same
> > *  email address you originally used to subscribe (do not
> > *  give an alias unless it was used to subscribe).
> > *
> > *  Visit http://www.techservinc.com/protelusers/subscrib.html
> > *  to unsubscribe or to subscribe a new email address.
> > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
>
>
> * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
> *  This message sent by: PROTEL EDA USERS MAILING LIST
> *
> *  Use the "reply" command in your email program to
> *  respond to this message.
> *
> *  To unsubscribe from this mailing list use the form at
> *  the Association web site. You will need to give the same
> *  email address you originally used to subscribe (do not
> *  give an alias unless it was used to subscribe).
> *
> *  Visit http://www.techservinc.com/protelusers/subscrib.html
> *  to unsubscribe or to subscribe a new email address.
> * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
>


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
*  This message sent by: PROTEL EDA USERS MAILING LIST
*
*  Use the "reply" command in your email program to
*  respond to this message.
*
*  To unsubscribe from this mailing list use the form at
*  the Association web site. You will need to give the same
*  email address you originally used to subscribe (do not
*  give an alias unless it was used to subscribe).
*
*  Visit http://www.techservinc.com/protelusers/subscrib.html
*  to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

________________________________________________________
To leave the EDAFORUM discussion list, send a email with
'leave edaforum' in the body to '[EMAIL PROTECTED]'

Reply via email to