Re: [PEDA] Find and Set Testpoints
I agree with Ian, the testpoint feature is pretty much useless. I also found the testpoint report to be incomplete and inaccurate. For those reasons, I have my customers generate a separate schematic page with nothing but testpoints. The clear advantages are you can control clearances, top or bottom sides, and have much better control over size and location. There is no easy method to do some tasks, this is one of them. Even the testpont generator in other programs like spectra doesn't work well either. It generates top test points under components which is not desirable.Using Ians method doesn't take long .I will complete a design, then add the testpoints after importing a netlist for the final time.Move component (testpoint) manually to desired locations is a cinch. Afterwards I use the pick and place output to generate their locations, merge is with a netlist report and it works everytime on all machines. Mike Reagan EDSI Frederick MD - Original Message - From: Ian Wilson [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Wednesday, August 21, 2002 6:25 PM Subject: Re: [PEDA] Find and Set Testpoints On 03:07 PM 21/08/2002 -0500, Michael Biggs said: What issues prevent Find and Set Testpoints - from converting connector pads or vias to be testpoints if your Testpoit style and Testpoit usage are all ok. I have to manually go and set the pads for testpoints and they are through holes. The design rules clear ok but why doesnt it pick up on all the vias and pads needed? Protel's testpoint finder is not really all that useful for current technology tester. It assumes that the points must be on a grid - most modern testers only require a certain separation (100mils preferred, 75 mils OK). I have had poor results with the Testpoint finder. The testpoint rule is great - it will alert my to any net without a testpoint. There is/was, I think an third party testpoint finder - it may (not sure) have been at: http://www.eda.co.uk We often have quite dense boards. We usually try to achieve 100% testpoint coverage. Although we prefer not to use a via as a test point, due to possible barrel damage, we do sometimes. Since the boards are dense we like to tent the top of the via but expose the bottom of those that are set as testpoints. P99SE did not allow selective top and bottom tenting (DXP does). So we manually placed a testpoint component (a simple 1mm round pad) over the vias that we want to expose as test point. The Sch has all the testpoints marked for debugging. The testpoint components can be placed on vias if necessary or nearby a via and a track run, if possible. A simple rule can be set to check clearances between testpoint components (we normally name the single pad as something like TP, within the library footprint and then set a Pad to pad clearance rule with a suitable scope based on the pad name. The testpoint component can include a 5mil wide, 47.5mil radius arc on a mech layer to show (visually) the clearance required. Since the testpoints are components they have automatic text (designator) that can be hidden or shown as desired, which matches the Sch. There are lots of advantages in this over using existing pads and vias as testpoint. In fact, the ability to be able to set a rule checking the distance between testpoint pads is missing unless you use a separate pad, or you use other contrived methods. We use Footprint-Pad scope - only out TP component (with its single TP pad) is used as a testpoint so the rule is easy). Can any one else come up with a clearance rule that checks that any via or pad marked as a testpoint (either free or within a component) is at least xyz mils from its nearest neighbour? Is is there anyway to select all the pads you want as testpoints and do a global edit? Mine was'nt working for me. Any thoughts? http://www.considered.com.au/Protel01.htm There is a freeware server there to allow this. In the past I used to do it (set the testpoint status of selected pads/vias) by saving-as an ASCII format and then using a search and replace to change the testpoint status as required for records marked as selected. I got sick of doing this hence the server. For some very unknown and unfathomable reason Altium did not permit global operations on the testpoint status. No idea why. It may be that the global code in P99Se was getting quite complex and any change required significant changes elsewhere - I can't imagine that it would be deliberately left out if it was easy to do. Ian Wilson * Tracking #: C6DAC609AD84274D8D85C98F600DC9C9E842FAA2 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http
Re: [PEDA] Find and Set Testpoints
Mike Ian, Yup another 100% agree, if a design requires test points I put them all as parts in the schematic otherwise the way Protel handles doing them from all aspects is pretty much absolutely useless from a design standpoint. I played around a bit early on to see if I could get something workable but no luck, if you want any kind of flexibility with test point, you have to bite the bullet and put them into the schematic. Bob Wolfe - Original Message - From: Michael Reagan (EDSI) [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Thursday, August 22, 2002 11:06 AM Subject: Re: [PEDA] Find and Set Testpoints I agree with Ian, the testpoint feature is pretty much useless. I also found the testpoint report to be incomplete and inaccurate. For those reasons, I have my customers generate a separate schematic page with nothing but testpoints. The clear advantages are you can control clearances, top or bottom sides, and have much better control over size and location. There is no easy method to do some tasks, this is one of them. Even the testpont generator in other programs like spectra doesn't work well either. It generates top test points under components which is not desirable.Using Ians method doesn't take long .I will complete a design, then add the testpoints after importing a netlist for the final time.Move component (testpoint) manually to desired locations is a cinch. Afterwards I use the pick and place output to generate their locations, merge is with a netlist report and it works everytime on all machines. Mike Reagan EDSI Frederick MD - Original Message - From: Ian Wilson [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Wednesday, August 21, 2002 6:25 PM Subject: Re: [PEDA] Find and Set Testpoints On 03:07 PM 21/08/2002 -0500, Michael Biggs said: What issues prevent Find and Set Testpoints - from converting connector pads or vias to be testpoints if your Testpoit style and Testpoit usage are all ok. I have to manually go and set the pads for testpoints and they are through holes. The design rules clear ok but why doesnt it pick up on all the vias and pads needed? Protel's testpoint finder is not really all that useful for current technology tester. It assumes that the points must be on a grid - most modern testers only require a certain separation (100mils preferred, 75 mils OK). I have had poor results with the Testpoint finder. The testpoint rule is great - it will alert my to any net without a testpoint. There is/was, I think an third party testpoint finder - it may (not sure) have been at: http://www.eda.co.uk We often have quite dense boards. We usually try to achieve 100% testpoint coverage. Although we prefer not to use a via as a test point, due to possible barrel damage, we do sometimes. Since the boards are dense we like to tent the top of the via but expose the bottom of those that are set as testpoints. P99SE did not allow selective top and bottom tenting (DXP does). So we manually placed a testpoint component (a simple 1mm round pad) over the vias that we want to expose as test point. The Sch has all the testpoints marked for debugging. The testpoint components can be placed on vias if necessary or nearby a via and a track run, if possible. A simple rule can be set to check clearances between testpoint components (we normally name the single pad as something like TP, within the library footprint and then set a Pad to pad clearance rule with a suitable scope based on the pad name. The testpoint component can include a 5mil wide, 47.5mil radius arc on a mech layer to show (visually) the clearance required. Since the testpoints are components they have automatic text (designator) that can be hidden or shown as desired, which matches the Sch. There are lots of advantages in this over using existing pads and vias as testpoint. In fact, the ability to be able to set a rule checking the distance between testpoint pads is missing unless you use a separate pad, or you use other contrived methods. We use Footprint-Pad scope - only out TP component (with its single TP pad) is used as a testpoint so the rule is easy). Can any one else come up with a clearance rule that checks that any via or pad marked as a testpoint (either free or within a component) is at least xyz mils from its nearest neighbour? Is is there anyway to select all the pads you want as testpoints and do a global edit? Mine was'nt working for me. Any thoughts? http://www.considered.com.au/Protel01.htm There is a freeware server there to allow this. In the past I used to do it (set the testpoint status of selected pads/vias) by saving-as an ASCII format and then using a search and replace to change the testpoint status as required for records marked as selected. I got sick of doing
[PEDA] Find and Set Testpoints
What issues prevent Find and Set Testpoints - from converting connector pads or vias to be testpoints if your Testpoit style and Testpoit usage are all ok. I have to manually go and set the pads for testpoints and they are through holes. The design rules clear ok but why doesnt it pick up on all the vias and pads needed? Is is there anyway to select all the pads you want as testpoints and do a global edit? Mine was'nt working for me. Any thoughts? Thanks MB * Tracking #: BD68386F9054F8489F38D39E8D33F777E547E362 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
