Re: [PEDA] How to highlight the Net in different colors in 99SE
If you select Tools|Preferences then the Display tab, there's a checkbox for 'Use Net Color For Highlight'. To set the net colours, on the 'Browse PCB' tab select 'Nets' on the dropdown. Scroll to the required net and click the Edit button. This brings up a Net Properties dialog where you can set the net colour. Once this is done, select both nets and the tracks will be highlighted in their own colours. Note that the highlight colour is the same for all layers, so not every 'near miss' will be genuine but it does help track them down. Regards, Andy Gulliver -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED] Sent: 28 February 2004 21:59 To: 'Protel EDA Forum' Subject: Re: [PEDA] How to highlight the Net in different colors in 99SE You can't because there is only one highlight color. If you had DXP you could filter by the two nets, such as (Net = 'A5') OR (Net = 'D0') and using the masking feature, these two nets are shows very clearly. Tony -Original Message- From: Adeel Malik [mailto:[EMAIL PROTECTED] Sent: Saturday, February 28, 2004 5:44 AM To: Protel EDA Forum Subject: [PEDA] How to highlight the Net in different colors in 99SE Hi All, I have a populated board which has two nets shorted to each other during assembly. I want to view both of the nets with different colors in Protel 99SE PCB document, so that I can locate the potential areas where the two nets are in close proximity. Can some one tell me how to view the two nets with different colors to solve the afore-mentioned problem in Protel 99SE ? Thanks, ADEEL MALIK * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] How to highlight the Net in different colors in 99SE
It seems as if this doesn't work in DXP. I checked 'Use Net Color For Highlight' and edited the color of a few nets, but when I highlight them they are still white. -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED] Sent: Monday, March 01, 2004 10:03 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] How to highlight the Net in different colors in 99SE Andy, that's brilliant! I don't think I ever knew about that feature!! That should fix him right up! I wonder how well it works in DXP with the masking??? -Original Message- From: Andy Gulliver [mailto:[EMAIL PROTECTED] Sent: Monday, March 01, 2004 2:44 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] How to highlight the Net in different colors in 99SE If you select Tools|Preferences then the Display tab, there's a checkbox for 'Use Net Color For Highlight'. To set the net colours, on the 'Browse PCB' tab select 'Nets' on the dropdown. Scroll to the required net and click the Edit button. This brings up a Net Properties dialog where you can set the net colour. Once this is done, select both nets and the tracks will be highlighted in their own colours. Note that the highlight colour is the same for all layers, so not every 'near miss' will be genuine but it does help track them down. Regards, Andy Gulliver -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED] Sent: 28 February 2004 21:59 To: 'Protel EDA Forum' Subject: Re: [PEDA] How to highlight the Net in different colors in 99SE You can't because there is only one highlight color. If you had DXP you could filter by the two nets, such as (Net = 'A5') OR (Net = 'D0') and using the masking feature, these two nets are shows very clearly. Tony -Original Message- From: Adeel Malik [mailto:[EMAIL PROTECTED] Sent: Saturday, February 28, 2004 5:44 AM To: Protel EDA Forum Subject: [PEDA] How to highlight the Net in different colors in 99SE Hi All, I have a populated board which has two nets shorted to each other during assembly. I want to view both of the nets with different colors in Protel 99SE PCB document, so that I can locate the potential areas where the two nets are in close proximity. Can some one tell me how to view the two nets with different colors to solve the afore-mentioned problem in Protel 99SE ? Thanks, ADEEL MALIK * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] How to highlight the Net in different colors in 99SE
that was the feature i was trying to suggest i thought it was in there but i couldn't remember it exactly right either thanks andy Dennis Saputelli Tony Karavidas wrote: Andy, that's brilliant! I don't think I ever knew about that feature!! That should fix him right up! I wonder how well it works in DXP with the masking??? -Original Message- From: Andy Gulliver [mailto:[EMAIL PROTECTED] Sent: Monday, March 01, 2004 2:44 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] How to highlight the Net in different colors in 99SE If you select Tools|Preferences then the Display tab, there's a checkbox for 'Use Net Color For Highlight'. To set the net colours, on the 'Browse PCB' tab select 'Nets' on the dropdown. Scroll to the required net and click the Edit button. This brings up a Net Properties dialog where you can set the net colour. Once this is done, select both nets and the tracks will be highlighted in their own colours. Note that the highlight colour is the same for all layers, so not every 'near miss' will be genuine but it does help track them down. Regards, Andy Gulliver -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED] Sent: 28 February 2004 21:59 To: 'Protel EDA Forum' Subject: Re: [PEDA] How to highlight the Net in different colors in 99SE You can't because there is only one highlight color. If you had DXP you could filter by the two nets, such as (Net = 'A5') OR (Net = 'D0') and using the masking feature, these two nets are shows very clearly. Tony -Original Message- From: Adeel Malik [mailto:[EMAIL PROTECTED] Sent: Saturday, February 28, 2004 5:44 AM To: Protel EDA Forum Subject: [PEDA] How to highlight the Net in different colors in 99SE Hi All, I have a populated board which has two nets shorted to each other during assembly. I want to view both of the nets with different colors in Protel 99SE PCB document, so that I can locate the potential areas where the two nets are in close proximity. Can some one tell me how to view the two nets with different colors to solve the afore-mentioned problem in Protel 99SE ? Thanks, ADEEL MALIK -- ___ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st StreetFax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] How to highlight the Net in different colors in 99SE
In a message dated 2/28/2004 4:17:26 PM Eastern Standard Time, [EMAIL PROTECTED] writes: I have a populated board which has two nets shorted to each other during assembly. I want to view both of the nets with different colors in Protel 99SE PCB document, so that I can locate the potential areas where the two nets are in close proximity. Can some one tell me how to view the two nets with different colors to solve the afore-mentioned problem in Protel 99SE ? BTDT. I usually do this by selecting one of the affected nets, which highlights the whole net. Then just click on a short segment of the other net, which will focus and highlight that net. The segment that you click will remain in the original color but show drag handles; the rest of the net will be highlighted. Good luck finding the short - I find this to be a very useful method of looking for it. I had to do this just last week. Took me about one minute to find the solder bridge under a microscope this way, because I only had about 3 places to look after a quick look at the board with the nets highlighted. Steve Hendrix * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] How to highlight the Net in different colors in 99SE
but you can make the nets different colors you just can't change the highlight color which i think is what he wanted just double click the net in browse PCB Dennis Saputelli Tony Karavidas wrote: You can't because there is only one highlight color. If you had DXP you could filter by the two nets, such as (Net = 'A5') OR (Net = 'D0') and using the masking feature, these two nets are shows very clearly. Tony -Original Message- From: Adeel Malik [mailto:[EMAIL PROTECTED] Sent: Saturday, February 28, 2004 5:44 AM To: Protel EDA Forum Subject: [PEDA] How to highlight the Net in different colors in 99SE Hi All, I have a populated board which has two nets shorted to each other during assembly. I want to view both of the nets with different colors in Protel 99SE PCB document, so that I can locate the potential areas where the two nets are in close proximity. Can some one tell me how to view the two nets with different colors to solve the afore-mentioned problem in Protel 99SE ? Thanks, ADEEL MALIK -- ___ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st StreetFax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] How to highlight the Net in different colors in 99SE
Hi Adeel, I would select one net and change it to an unused layer, with its own colour, then do the same for the other net. Although I have always found shorts using a ohm meter on a milli-ohm scale, you can narrow it down to a small area very quickly. Darren Moore -Original Message- From: Adeel Malik [mailto:[EMAIL PROTECTED] Hi All, I have a populated board which has two nets shorted to each other during assembly. I want to view both of the nets with different colors in Protel 99SE PCB document, so that I can locate the potential areas where the two nets are in close proximity. Can some one tell me how to view the two nets with different colors to solve the afore-mentioned problem in Protel 99SE ? Thanks, ADEEL MALIK * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] How to highlight the Net in different colors in 99SE
True, but changing the net color would only change the ratsnets. He already has a routed board with a short somewhere. DXP would help him see it. -Original Message- From: Dennis Saputelli [mailto:[EMAIL PROTECTED] Sent: Saturday, February 28, 2004 4:48 PM To: Protel EDA Forum Subject: Re: [PEDA] How to highlight the Net in different colors in 99SE but you can make the nets different colors you just can't change the highlight color which i think is what he wanted just double click the net in browse PCB Dennis Saputelli Tony Karavidas wrote: You can't because there is only one highlight color. If you had DXP you could filter by the two nets, such as (Net = 'A5') OR (Net = 'D0') and using the masking feature, these two nets are shows very clearly. Tony -Original Message- From: Adeel Malik [mailto:[EMAIL PROTECTED] Sent: Saturday, February 28, 2004 5:44 AM To: Protel EDA Forum Subject: [PEDA] How to highlight the Net in different colors in 99SE Hi All, I have a populated board which has two nets shorted to each other during assembly. I want to view both of the nets with different colors in Protel 99SE PCB document, so that I can locate the potential areas where the two nets are in close proximity. Can some one tell me how to view the two nets with different colors to solve the afore-mentioned problem in Protel 99SE ? Thanks, ADEEL MALIK -- __ _ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st StreetFax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *