Re: [PEDA] adjacent component placement DXP
On 06:45 PM 9/07/2003, Jason Morgan said:
Firstly you posted to the wrong list, this list is for Protel 99se, and not
DXP,
there is a separate list for DXP issues, see
http://forums.altium.com/cgi-bin/msgbylist.asp?list=dxp
PEDA is not just for P99SE but is certainly mainly used for that - the
Altium DXP list certainly has a much higher SNR both generally and for DXP
related stuff.
To answer your question, its the same as in 99se, you create a
component-component clearance rule
that uses the same component type for each side of the rule.
I use this exact method for a mechanical part that sits over some LEDs.
e.g.
Create a rule in Placement: Component Clearance: New Rule
HasFootprint('FOOTPRINT_1') vs HasFootprint('FOOTPRINT_1') you need to
specify Full Check
and a large negative clearance, e.g. -999mm
My experience is that this doesn't work. DXP does not support negative
clearance checking (overlaps). It has been something I and others have
been asking for for a while now. I just tried a test case and couldn't get
it to pass a batch DRC if I had any overlap at all - a negative clearance
acted like a zero clearance.
Are you sure this has worked for you, Jason. Can you give a little more
detail? I would love to know why it doesn't work for me.
The only way I have been able to solve this sort of problem is by excluding
the affected footprint from testing by making the general (All-All) rule
into a:
NOT HasFootprint('FOOTPRINT_1') vs NOT HasFootprint('FOOTPRINT_1')
This excludes 'FOOTPRINT_1', in this case, from any clearance checking -
but this then means that *no* component is checked against any component
with footprint 'FOOTPRINT_1'. I thought I had solved this issue to exclude
just 'FOOTPRINT_1' from being checked against any other 'FOOTPRINT_1' but
all other components being checked against each other and 'FOOTPRINT_1' but
I can't recall and it is late. I think there should be something in the
DXP forum archive on this.
This solution is pretty poor as it doesn't scale well. A number of users
have been requesting generalised clearance rules (not just component and
electrical) with negative clearance (overlap) capability. Hopefully it
will appear in a DXP SP soon.
Ian
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] adjacent component placement DXP
Ian,
I can state that it works for me - honest. The area of the PCB in question
is over 2 years old - obviously inherited from 99se.
In this case, the components in question are an array of LEDs with a light
pipe over them, all tightly
packed together.
I've not experimented with the actual parameters in DXP, but I know 'full
checking' MUST be on and I recall
having to play with the negative clearance in 99se, ending up at -127mm.
IIRC The online DRC always fails - annoyingly - but a full DRC passes with
this rule in place.
If I find time I'll take a look at it and see if I can work out *WHY* it
works.
It seems that this method perhaps does not work in all cases, at least
without some messing and plain luck.
I agree on the generalised clearance rule. Hm, perhaps this conversation
should be on DXP as it seems a little product enhancement is in order ;)
J.
-Original Message-
From: Ian Wilson [mailto:[EMAIL PROTECTED]
Sent: 09 July 2003 12:59
To: Protel EDA Forum
Cc: DXP Technical Forum
Subject: Re: [PEDA] adjacent component placement DXP
On 06:45 PM 9/07/2003, Jason Morgan said:
Firstly you posted to the wrong list, this list is for Protel 99se, and not
DXP,
there is a separate list for DXP issues, see
http://forums.altium.com/cgi-bin/msgbylist.asp?list=dxp
PEDA is not just for P99SE but is certainly mainly used for that - the
Altium DXP list certainly has a much higher SNR both generally and for DXP
related stuff.
To answer your question, its the same as in 99se, you create a
component-component clearance rule
that uses the same component type for each side of the rule.
I use this exact method for a mechanical part that sits over some LEDs.
e.g.
Create a rule in Placement: Component Clearance: New Rule
HasFootprint('FOOTPRINT_1') vs HasFootprint('FOOTPRINT_1') you need to
specify Full Check
and a large negative clearance, e.g. -999mm
My experience is that this doesn't work. DXP does not support negative
clearance checking (overlaps). It has been something I and others have
been asking for for a while now. I just tried a test case and couldn't get
it to pass a batch DRC if I had any overlap at all - a negative clearance
acted like a zero clearance.
Are you sure this has worked for you, Jason. Can you give a little more
detail? I would love to know why it doesn't work for me.
The only way I have been able to solve this sort of problem is by excluding
the affected footprint from testing by making the general (All-All) rule
into a:
NOT HasFootprint('FOOTPRINT_1') vs NOT HasFootprint('FOOTPRINT_1')
This excludes 'FOOTPRINT_1', in this case, from any clearance checking -
but this then means that *no* component is checked against any component
with footprint 'FOOTPRINT_1'. I thought I had solved this issue to exclude
just 'FOOTPRINT_1' from being checked against any other 'FOOTPRINT_1' but
all other components being checked against each other and 'FOOTPRINT_1' but
I can't recall and it is late. I think there should be something in the
DXP forum archive on this.
This solution is pretty poor as it doesn't scale well. A number of users
have been requesting generalised clearance rules (not just component and
electrical) with negative clearance (overlap) capability. Hopefully it
will appear in a DXP SP soon.
Ian
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] adjacent component placement DXP
Hi all, Need to place a number of terminal blocks in a row, with the body of each touching that of its neighbour, on a PCB being laid out in Protel DXP. Despite setting the electrical placement and component clearance DRCs for these particular components to 0mm, Protel still flags this a violation when they are placed next to each other. . Anyone come across this problem/know of a workaround? Many thanks Gwyn Roberts Univ of Wales, Bangor * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] adjacent component placement DXP
Firstly you posted to the wrong list, this list is for Protel 99se, and not
DXP,
there is a separate list for DXP issues, see
http://forums.altium.com/cgi-bin/msgbylist.asp?list=dxp
To answer your question, its the same as in 99se, you create a
component-component clearance rule
that uses the same component type for each side of the rule.
I use this exact method for a mechanical part that sits over some LEDs.
e.g.
Create a rule in Placement: Component Clearance: New Rule
HasFootprint('FOOTPRINT_1') vs HasFootprint('FOOTPRINT_1') you need to
specify Full Check
and a large negative clearance, e.g. -999mm
Make sure that the rule priority puts this rule above the global clearance
rule, Press the Priorities
button to check.
Also, make sure that one of the electrical clearance rules does not also
fail, though you should be
able to tell the difference of a component clearance fail and a net fail by
the colours on the screen.
Jason.
-Original Message-
From: Dr Gwyn Roberts [mailto:[EMAIL PROTECTED]
Sent: 09 July 2003 09:21
To: [EMAIL PROTECTED]
Cc: Aled Williams
Subject: [PEDA] adjacent component placement DXP
Hi all,
Need to place a number of terminal blocks in a row, with the body of
each touching that of its neighbour, on a PCB being laid out in Protel DXP.
Despite setting the electrical placement and component clearance DRCs
for these particular components to 0mm, Protel still flags this a
violation when they are placed next to each other. .
Anyone come across this problem/know of a workaround?
Many thanks
Gwyn Roberts
Univ of Wales, Bangor
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] adjacent component placement DXP
The very same thing in 98SE made me quite cross. There is probably a right way to fix this. I couldn't find it and turned off the component clearance rule instead. Dr Gwyn Roberts [EMAIL PROTECTED]To: [EMAIL PROTECTED] ngor.ac.uk cc: Aled Williams [EMAIL PROTECTED] Subject: [PEDA] adjacent component placement DXP 09-Jul-2003 09:20 AM Please respond to Protel EDA Forum Hi all, Need to place a number of terminal blocks in a row, with the body of each touching that of its neighbour, on a PCB being laid out in Protel DXP. Despite setting the electrical placement and component clearance DRCs for these particular components to 0mm, Protel still flags this a violation when they are placed next to each other. . Anyone come across this problem/know of a workaround? Many thanks Gwyn Roberts Univ of Wales, Bangor * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] adjacent component placement DXP
Dr Gwyn Roberts wrote: Hi all, Need to place a number of terminal blocks in a row, with the body of each touching that of its neighbour, on a PCB being laid out in Protel DXP. Despite setting the electrical placement and component clearance DRCs for these particular components to 0mm, Protel still flags this a violation when they are placed next to each other. . Anyone come across this problem/know of a workaround? Many thanks Gwyn Roberts Univ of Wales, Bangor One solution is to draw the component outline of these parts slightly undersize. For example, for 1/4W resistors that I want to place on 0.1 inch centers, I make the component outline 0.090 wide - then, even with .01 wide tracks for the outline, the outlines will not overlap. -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
