Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
Yes and No. Yes I designed the board and No the Vias are not free pads. There is no holes in the solder paste layers on the origional protel drawing, only on the gerber import. The gerber import is just photoplot commands, therefore if there is a shape there then there will be a hole. J. -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: 18 February 2002 19:31 To: 'Protel EDA Forum' Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask Jason, did you actually design this board? Because I have a feeling that what you're describing means that your vias are actually free pads. Is that a possibility? Normally vias don't show on a solderpaste layer. Other possiblity is that you have loaded a padmaster back in as a pastemask. I have assumed that in your original message you were trying to say ...tented vias have solder paste on them from the paste mask layer. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. Microwave Products Tel (604) 292-9089 (direct line) Fax (604) 292-9010 email: [EMAIL PROTECTED] http://www.norsat.com See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]] Sent: Monday, February 18, 2002 10:58 AM To: Protel EDA Forum Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask In a message dated 2/18/2002 1:42:56 PM Eastern Standard Time, [EMAIL PROTECTED] writes: As normal we load the gerbers back into protel to check they look right, I've noticed that the tented vias have solder on them on the paste mask. Why, and how do I get rid of it? I've never noticed this before but can't say it hasn't happened. We're just about to spin the boards and want to know if this will affect the mask manufacture. If so, I'd consider that a bug in Protel. But you may have been covered (so to speak) by the board house in the past. The board houses I've dealt with routinely mask the silkscreen with the soldermask layer, so you don't get ink on the exposed pads. The assembly house may well do the same thing between the soldermask and the paste mask, to avoid getting past on top of the soldermask. If so, that would explain why you haven't seen a problem in the past. 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/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
Entirely probable.. We sent the gerbers anyway. And then tried a different gerber viewer this morning. PANIC OVER, call off the dogs. Leon was right. Protels' importer saw the vias as through hole pads, so placed a free pad at its location on multi layer. The free pads have a paste mask so protel created one in addition to the paste mask that was in the gerber. Not sure if that is actually a bug, probably not, but something to be aware of. Many thanks, Jason -Original Message- From: ICT Mail [mailto:[EMAIL PROTECTED]] Sent: 18 February 2002 23:43 To: Protel EDA Forum Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask Jason, just a thought here When you load gerbers back into a blank PCB file, you must remember that for a given layer, all the lands that represent vias and pads etc will be imported as free pads and will take on the design rules specified in your PCB file. Vias are just a D-code for a given artwork layer. I suspect that if you tented these vias when looking at them in Protel after importing the gerbers, they would actually have a Solder Mask assigned which would be the default for a free pad or general rule in the viewing PCB file. I would recommend using a Gerber viewer / editor for viewing Gerber files. Leon Fonstin -Original Message- From: Jason Morgan [mailto:[EMAIL PROTECTED]] Sent: Tuesday, 19 February 2002 5:36 AM To: Protel EDA Forum (E-mail) Subject: [PEDA] URGENT HELP REQUIRED: Paste Mask Importance: High Hi, As normal we load the gerbers back into protel to check they look right, I've noticed that the tented vias have solder on them on the paste mask. Why, and how do I get rid of it? I've never noticed this before but can't say it hasn't happened. We're just about to spin the boards and want to know if this will affect the mask manufacture. Many thanks, Jason. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
Jason, if you haven't caught on to your problem yet, I think that one of the other posters hit the nail on the head. There may be nothing wrong with your original Gerber files, the problem may have arose when you imported them back into Protel. Importing Gerber back into Protel is something that I do not do, I want independent confirmation that the Gerbers are correctly generated. So if I don't do this explanation justice, bear with me and try to understand the concept I am pointing out. I believe that when you import Gerbers back into Protel then most of the imported pads are treated as free-pads upon importation. This new free-pad is not a via any longer (if it was a via pad to start with), now it is interpreted as a free pad and as such it will show a solderpaste mask opening in the database which you have imported it into. Remember that your imported Gerber is now a new Protel primitive and thus it may behave like any other primitive and may not truly represent the former Gerber element that you thought you imported. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. Microwave Products Tel (604) 292-9089 (direct line) Fax (604) 292-9010 email: [EMAIL PROTECTED] http://www.norsat.com See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Jason Morgan [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 19, 2002 1:08 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask Yes and No. Yes I designed the board and No the Vias are not free pads. There is no holes in the solder paste layers on the origional protel drawing, only on the gerber import. The gerber import is just photoplot commands, therefore if there is a shape there then there will be a hole. J. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
Jason, I did not follow this one from the very beginning but, I would also 100% agree that bringing a gerber file back into your CAD system for any reason other than to use it to reproduce a board you have no CAD data for, or copy sections into an existing board etc. is not good. I would NOT recommend it as a means of verifying gerber data for fabrication. Way back Cadnetix offered gerber import as the only means of checking gerbers too, but this was really not an accurate way to do this you really need to view them in another piece of sofware, which we did. Cadnetix also offered a smart gerber input for just the purpose of bringing a gerber only design into the CAD system. In all the cases I have seen like here with Protel bringing the gerber file into the CAD system usually relies on settings or pad data inherent from the CAD system. In the case of Cadnetix you were merely importing the pads from your own library to view up the gerber, an dbeliev me that is not checking any gerber data, it merely means you had a pad in the library with the proper name. In this case it seems its a problem with the way the CAD system handles vias. In any case use a separate viewer or CAM software to do this function. Bob Robert M. Wolfe, C.I.D. [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] URGENT HELP REQUIRED: Paste Mask
Hi, As normal we load the gerbers back into protel to check they look right, I've noticed that the tented vias have solder on them on the paste mask. Why, and how do I get rid of it? I've never noticed this before but can't say it hasn't happened. We're just about to spin the boards and want to know if this will affect the mask manufacture. Many thanks, Jason. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
Jason, did you actually design this board? Because I have a feeling that what you're describing means that your vias are actually free pads. Is that a possibility? Normally vias don't show on a solderpaste layer. Other possiblity is that you have loaded a padmaster back in as a pastemask. I have assumed that in your original message you were trying to say ...tented vias have solder paste on them from the paste mask layer. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. Microwave Products Tel (604) 292-9089 (direct line) Fax (604) 292-9010 email: [EMAIL PROTECTED] http://www.norsat.com See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]] Sent: Monday, February 18, 2002 10:58 AM To: Protel EDA Forum Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask In a message dated 2/18/2002 1:42:56 PM Eastern Standard Time, [EMAIL PROTECTED] writes: As normal we load the gerbers back into protel to check they look right, I've noticed that the tented vias have solder on them on the paste mask. Why, and how do I get rid of it? I've never noticed this before but can't say it hasn't happened. We're just about to spin the boards and want to know if this will affect the mask manufacture. If so, I'd consider that a bug in Protel. But you may have been covered (so to speak) by the board house in the past. The board houses I've dealt with routinely mask the silkscreen with the soldermask layer, so you don't get ink on the exposed pads. The assembly house may well do the same thing between the soldermask and the paste mask, to avoid getting past on top of the soldermask. If so, that would explain why you haven't seen a problem in the past. 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/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
At 06:36 PM 2/18/2002 +, you wrote: As normal we load the gerbers back into protel to check they look right, I've noticed that the tented vias have solder on them on the paste mask. Why, and how do I get rid of it? (1) are you sure that they are vias and not free pads? (2) what are the paste mask rule settings? We're just about to spin the boards and want to know if this will affect the mask manufacture. Paste mask is typically the last operation which might or might not give you a little extra time. It might even be applied by the assembler as distinct from the board fabricator [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] URGENT HELP REQUIRED: Paste Mask
Jason, just a thought here When you load gerbers back into a blank PCB file, you must remember that for a given layer, all the lands that represent vias and pads etc will be imported as free pads and will take on the design rules specified in your PCB file. Vias are just a D-code for a given artwork layer. I suspect that if you tented these vias when looking at them in Protel after importing the gerbers, they would actually have a Solder Mask assigned which would be the default for a free pad or general rule in the viewing PCB file. I would recommend using a Gerber viewer / editor for viewing Gerber files. Leon Fonstin -Original Message- From: Jason Morgan [mailto:[EMAIL PROTECTED]] Sent: Tuesday, 19 February 2002 5:36 AM To: Protel EDA Forum (E-mail) Subject: [PEDA] URGENT HELP REQUIRED: Paste Mask Importance: High Hi, As normal we load the gerbers back into protel to check they look right, I've noticed that the tented vias have solder on them on the paste mask. Why, and how do I get rid of it? I've never noticed this before but can't say it hasn't happened. We're just about to spin the boards and want to know if this will affect the mask manufacture. Many thanks, Jason. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
