Re: [PEDA] Copy selection to layer
Thanks Jim, You are a font of information. I disabled Optimize Wires and Busses, and now it looks like good ol' Protel again. Hopefully this won't come back to bite me later with connectivity issues... Bob -Original Message- From: Jim Monroe [mailto:[EMAIL PROTECTED] Sent: Monday, August 09, 2004 12:45 PM To: Protel EDA Forum Subject: Re: [PEDA] Copy selection to layer Bob- Again I'll assume you are wanting to move the end of a wire in DXP. Try Edit/Break Wire and Move/Drag. The default operation of DXP now automatically joins wires (unless you disable Optimize Wires), so if you draw a short wire then continue a new wire at the end of the old, the two become one. You cannot move the end of the first wire because it no longer exists. You can however clip a section out of the middle of the wire using the Break Wire command, creating two separate wire. Then click to wire to select it and show its handles, then use the Move/Drag command or simply click and drag one of the handles. The 2nd chapter in the Manual gives a good tutorial on the basics for Schematic and PCB. If you have the DXP04 upgrade that didn't come with paper manuals, you can get it in PDF format in the Altium\Protel2004 folder in your program directory or from the web at http://www.altium.com/learningguides/TU0117_GettingStartedWithPCBDesign.pdf. JM At 06:17 AM 8/9/2004, you wrote: Thanks Jim. That's a big help. Is there a similar command for trimming wires in schematics? Bob -Original Message- From: Jim Monroe [mailto:[EMAIL PROTECTED] Sent: Friday, August 06, 2004 5:12 PM To: Protel EDA Forum Subject: Re: [PEDA] Copy selection to layer Bob- Are you talking about moving the end of a trace? If so, the shortcut was Ctrl + LeftClick. DXP still has this capability by using the move drag end command but shortcut doesn't work anymore, it was reassigned to highlight net. You can re-assign the shortcut back to the Move/Drag command or give it a new shortcut. I have a favorite little know trick that did make the transition intact. Excess length of track stubs can be trimmed simply by double clicking while Interactive Routing (Automatically Remove Loops must be enabled). The stub beyond the double click point instantly disappears. Having the electrical snap enabled also helps. BTW, I'm trying to figure out which DXP shortcut keys are not yet used. Does anyone know if it is possible to list shortcuts sorted by keystroke? This was another easy task in 99se that isn't so apparent in DXP. JM At 06:22 AM 8/6/2004, bob stephens wrote: Another feature I really miss is the ability to trim or shorten a PCB trace by some combination of shift/ctrl/click/drag which I forget. I can't fathom why they would get rid of this very useful feature... * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Orcad schem part field for TOPSIDE or BOTTSIDE
On 03:07 AM 10/08/2004, Dennis Saputelli said: Orcad Capture has a schem part field for TOPSIDE or BOTTSIDE is there a way in 99SE or P2004 to get the netlist to dump the part on the indicated side of the board ? No, not automatically. You could use a part field (99SE) or a parameter (DXP/P2004) to indicate what side and then select and change globally - you would need a method to select components in the PCB based on what is selected in the Sch - can this be done in P99SE? (P2004 has a command to select PCB components based on what is selected in Sch, it works for components selected on multiple sheets. I can't recall if P99SE has this.) A script could do the layer flip in P2004 (iterate over all components and flip any that are on the wrong layer compared to the parameter/part field). Not sure if a macro could do it in P99SE, it may be able to but macro functionality is quite limited. A server could do it in P99SE. There are some tricks as you would need to deal with of course as the PCB components do not carry the part fields/parameters so you need to go back and compare with the Sch or the netlist. 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] Orcad schem part field for TOPSIDE or BOTTSIDE
seems like this would be possibly a nice feature to optionally control from the schematic and be fully automatic if you didn't like the result you could still muck about with the parts selectively Orcad capture also has what i think is a new feature to v. 10: a big spreadsheet type panel with all the objects across all the sheets which can be sorted by their columns and which can be used to globally edit things reasonably simply Dennis Saputelli Ian Wilson wrote: On 03:07 AM 10/08/2004, Dennis Saputelli said: Orcad Capture has a schem part field for TOPSIDE or BOTTSIDE is there a way in 99SE or P2004 to get the netlist to dump the part on the indicated side of the board ? No, not automatically. You could use a part field (99SE) or a parameter (DXP/P2004) to indicate what side and then select and change globally - you would need a method to select components in the PCB based on what is selected in the Sch - can this be done in P99SE? (P2004 has a command to select PCB components based on what is selected in Sch, it works for components selected on multiple sheets. I can't recall if P99SE has this.) A script could do the layer flip in P2004 (iterate over all components and flip any that are on the wrong layer compared to the parameter/part field). Not sure if a macro could do it in P99SE, it may be able to but macro functionality is quite limited. A server could do it in P99SE. There are some tricks as you would need to deal with of course as the PCB components do not carry the part fields/parameters so you need to go back and compare with the Sch or the netlist. Ian -- ___ 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] Orcad schem part field for TOPSIDE or BOTTSIDE
On 10:31 AM 11/08/2004, Dennis Saputelli said: seems like this would be possibly a nice feature to optionally control from the schematic and be fully automatic if you didn't like the result you could still muck about with the parts selectively Yep. I agree. Users have been suggesting a number of things (on the DXP forum) that increase the ability to control layout from sch. Things like setting layers and being able to create classes (nets, components etc) in the sch. Maybe some of these ideas will appear at some stage. Orcad capture also has what i think is a new feature to v. 10: a big spreadsheet type panel with all the objects across all the sheets which can be sorted by their columns and which can be used to globally edit things reasonably simply Sort of like DXP/P2004's List panel is it? P99SE has this but you have to export-change-import and this is a somewhat fiddly process. One of my dislikes about P2004 is that the List panel is always active (even if not visible). The List panel is great when necessary but filling it and emptying it *might* be a cause of delays when doing queries that affect lots of objects - there are delays but us users are not privy to all the causes, I hypothesize that the List panel is one cause. I say might as there is no way of confirming whether this is the case, but it is a possibility. However there are times when the List panel is very useful. You can sort by clicking on column headers. You can edit a bunch of objects at the same time. You can show child objects of group objects (polygons, components etc). Managing the columns that are shown could be better I think. The List, like the Inspector, by default only shows columns that are common to all the objects returned by the current filter. So when no filter is active it shows everything and so you don't have many useful columns - you can turn on more columns manually. The main issue I have with P2004 implementation of the List panel (spreadsheet view) is that keeping it up-to-date is possibly a cause of these pregnant pauses that one gets while running some queries/filters. I would like to be able to turn off the List panel so it is not having to be continually kept synched with the current filters. 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] Orcad schem part field for TOPSIDE or BOTTSIDE
In the case of this new orcad feature you specifically do it 'outside' of the graphical sch you point to sheets and it gathers a properties page kind of like a batch process ds Ian Wilson wrote: On 10:31 AM 11/08/2004, Dennis Saputelli said: seems like this would be possibly a nice feature to optionally control from the schematic and be fully automatic if you didn't like the result you could still muck about with the parts selectively Yep. I agree. Users have been suggesting a number of things (on the DXP forum) that increase the ability to control layout from sch. Things like setting layers and being able to create classes (nets, components etc) in the sch. Maybe some of these ideas will appear at some stage. Orcad capture also has what i think is a new feature to v. 10: a big spreadsheet type panel with all the objects across all the sheets which can be sorted by their columns and which can be used to globally edit things reasonably simply Sort of like DXP/P2004's List panel is it? P99SE has this but you have to export-change-import and this is a somewhat fiddly process. One of my dislikes about P2004 is that the List panel is always active (even if not visible). The List panel is great when necessary but filling it and emptying it *might* be a cause of delays when doing queries that affect lots of objects - there are delays but us users are not privy to all the causes, I hypothesize that the List panel is one cause. I say might as there is no way of confirming whether this is the case, but it is a possibility. However there are times when the List panel is very useful. You can sort by clicking on column headers. You can edit a bunch of objects at the same time. You can show child objects of group objects (polygons, components etc). Managing the columns that are shown could be better I think. The List, like the Inspector, by default only shows columns that are common to all the objects returned by the current filter. So when no filter is active it shows everything and so you don't have many useful columns - you can turn on more columns manually. The main issue I have with P2004 implementation of the List panel (spreadsheet view) is that keeping it up-to-date is possibly a cause of these pregnant pauses that one gets while running some queries/filters. I would like to be able to turn off the List panel so it is not having to be continually kept synched with the current filters. Ian -- ___ 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] footprint clearance checking
I have a connector that could be viewed as a large U when placed on the board. If I want to place other components within this U shape (not overlapping the physical connector but within the bounding box) what choices do I have: - permanently enjoying the 20+ clearance errors? (not preferred) - turning off clearance checking? (not preferred) - turning off clearance checking for that one connector whilst in that position (how?)? ( P2004 ) = Dom Bragge CID Snr PCB Designer Sydney, Australia Find local movie times and trailers on Yahoo! Movies. http://au.movies.yahoo.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] footprint clearance checking
Design it like all of the components in my publicly available library, where the silkscreen defines the outer inner edges of where the component surfaces meet the PCB. Shrink the component-component clearance to 1 mil, or 0 mil. This will allow you place, for example, some caps resistors right up to under some areas of a large PCB mounted RCA jack, but, it will not allow you to place components too close where the silk screen area may touch each other. Note that my library was intentionally designed like this for creating hand-held electronic devices where mounting area may be super constrictive. _ Brian Guralnick - Original Message - From: Dom Bragge To: Protel EDA forum Sent: Tuesday, August 10, 2004 11:10 PM Subject: [PEDA] footprint clearance checking I have a connector that could be viewed as a large U when placed on the board. If I want to place other components within this U shape (not overlapping the physical connector but within the bounding box) what choices do I have: - permanently enjoying the 20+ clearance errors? (not preferred) - turning off clearance checking? (not preferred) - turning off clearance checking for that one connector whilst in that position (how?)? ( P2004 ) = Dom Bragge CID Snr PCB Designer Sydney, Australia Find local movie times and trailers on Yahoo! Movies. http://au.movies.yahoo.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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
