Re: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5......
> I was just in the process of going over some gerbers for our latest board > design. I was looking at Mid Layer 1, where in my design I have placed > circular traces (8 mil wide tied to a internal ground plane with 30 mil > diameter pad with a 15 mil hole) around areas where summing junctions of OP > Amps pass from the top of the board to the bottom of the board. > > I noticed that in some cases there were some pads missing. Some of these > guards have pads connecting them to an internal plane and some just have a > drill hit. No pad what so ever. The pads are there in all cases when I > look at the PCB in Protel. > > Has any one else seen this phenomenon? Shouldn't there be a pad everywhere > there is a trace that passes through the board even on in internal signal > layer? > > John Branthoover I suspect that the option of including unconnected mid layer pads has not been selected. I don't have Protel 99 SE open at present, but in the CAM Manager server, the dialog box provided for setting up Gerber files has a number of tabs, and on one of those, there is a checkbox provided for controlling that setting. Check that checkbox and then re-generate your Gerber files. Regards, Geoff Harland. - E-Mail Disclaimer The Information in this e-mail is confidential and may be legally privileged. It is intended solely for the addressee. Access to this e-mail by anyone else is unauthorised. If you are not the intended recipient, any disclosure, copying, distribution or any action taken or omitted to be taken in reliance on it, is prohibited and may be unlawful. Any opinions or advice contained in this e-mail are confidential and not for public display. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5......
Yes with 99SE and SP5 I have seen inner layer gerbers with a pad missing. Luckily this was spotted during error checking of Gerbers by our PCB manufacturer and the missing pad added at Gerber level. No matter how hard we tried we could not get the pad to appear. Even trying different machines and setups, pad missing. Using SP6 though all pads present. So update to SP6 and try again. regards Ian > -Original Message- > From: John Branthoover [mailto:[EMAIL PROTECTED]] > Sent: 29 March 2001 21:58 > To: [EMAIL PROTECTED] > Subject: [PEDA] Problems With Gerbers Generated With Protel 99SE > SP5.. > > > Hello all, > I was just in the process of going over some gerbers for > our latest board > design. I was looking at Mid Layer 1, where in my design I have placed > circular traces (8 mil wide tied to a internal ground plane with 30 mil > diameter pad with a 15 mil hole) around areas where summing > junctions of OP > Amps pass from the top of the board to the bottom of the board. > > I noticed that in some cases there were some pads missing. > Some of these > guards have pads connecting them to an internal plane and some just have a > drill hit. No pad what so ever. The pads are there in all cases when I > look at the PCB in Protel. > > Has any one else seen this phenomenon? Shouldn't there be > a pad everywhere > there is a trace that passes through the board even on in internal signal > layer? > > Thank you for your time and have a nice day. > > > > John Branthoover: > Electrical Design Engineer : > Acutronic R & D:Phone (412) 968-1051 > 137/139 Delta Drive :Fax(412) 963-0519 > Pittsburgh PA 15238 :Email [EMAIL PROTECTED] > USA :WEBhttp://www.acutronic.com > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5......
At 03:58 PM 3/29/01 -0500, John Branthoover wrote: > Has any one else seen this phenomenon? Shouldn't there be a pad > everywhere >there is a trace that passes through the board even on in internal signal >layer? Glad you asked. (Others have already answered but I may have another slant on the matter.) I hadn't looked into this matter since Protel 98. In Protel 98, connectivity of an arc was only established at the arc endpoints. So if you plopped a via down onto the arc where it did not touch an endpoint (a full arc still has a single endpoint), the via would not pick up the arc's net. This explains why dead pad removal on Gerbers did not plot that pad, and likewise why they would not connect to an inner plane. The via had no net assignment. If you manually edited the via to the proper net, or placed it in contact with a primitive of the proper net (including an arc endpoint) and then move it to its final position, it would have worked. I'm not sure about DRC, but the plots would be correct. Apparently this has been fixed in SP6: I just verified that a via dropped anywhere on an arc picks up the net. [EMAIL PROTECTED] Abdulrahman Lomax P.O. Box 690 El Verano, CA 95433 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5......
Hello Bob, Yes, you have hit the problem right on the head. When a pad or via is placed on a arc in Protel 99SE SP5, It does not generate a pad on the inner layers. Placing a small track on the pad solves this problem. In my case I just removed the arcs, I only had a few to take care of. I will have to look into upgrading to SP6. Thank you again gentlemen for you help. Have a nice day.! -Original Message- From: BOB JONES [mailto:[EMAIL PROTECTED]] Sent: Monday, April 02, 2001 4:28 PM To: Protel EDA Forum Subject: Re: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5.. I'm wondering if the missing pads are ones that end on an arc? I've seen this with SP5, any trace that ends in an arc and has a via at the end will not show up on mid layers on the gerbers. SP6 supposedly fixes this. A fix for SP5 is to add a small trace (one that doesn't go past the via) on the same layer as the arc. This has worked for me. - Original Message - From: "John Branthoover" <[EMAIL PROTECTED]> To: <[EMAIL PROTECTED]> Sent: Thursday, March 29, 2001 4:58 PM Subject: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5.. > Hello all, > I was just in the process of going over some gerbers for our latest board > design. I was looking at Mid Layer 1, where in my design I have placed > circular traces (8 mil wide tied to a internal ground plane with 30 mil > diameter pad with a 15 mil hole) around areas where summing junctions of OP > Amps pass from the top of the board to the bottom of the board. > > I noticed that in some cases there were some pads missing. Some of these > guards have pads connecting them to an internal plane and some just have a > drill hit. No pad what so ever. The pads are there in all cases when I > look at the PCB in Protel. > > Has any one else seen this phenomenon? Shouldn't there be a pad everywhere > there is a trace that passes through the board even on in internal signal > layer? > > Thank you for your time and have a nice day. > > > > John Branthoover: > Electrical Design Engineer : > Acutronic R & D:Phone (412) 968-1051 > 137/139 Delta Drive :Fax(412) 963-0519 > Pittsburgh PA 15238 :Email [EMAIL PROTECTED] > USA :WEBhttp://www.acutronic.com > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5......
I'm wondering if the missing pads are ones that end on an arc? I've seen this with SP5, any trace that ends in an arc and has a via at the end will not show up on mid layers on the gerbers. SP6 supposedly fixes this. A fix for SP5 is to add a small trace (one that doesn't go past the via) on the same layer as the arc. This has worked for me. - Original Message - From: "John Branthoover" <[EMAIL PROTECTED]> To: <[EMAIL PROTECTED]> Sent: Thursday, March 29, 2001 4:58 PM Subject: [PEDA] Problems With Gerbers Generated With Protel 99SE SP5.. > Hello all, > I was just in the process of going over some gerbers for our latest board > design. I was looking at Mid Layer 1, where in my design I have placed > circular traces (8 mil wide tied to a internal ground plane with 30 mil > diameter pad with a 15 mil hole) around areas where summing junctions of OP > Amps pass from the top of the board to the bottom of the board. > > I noticed that in some cases there were some pads missing. Some of these > guards have pads connecting them to an internal plane and some just have a > drill hit. No pad what so ever. The pads are there in all cases when I > look at the PCB in Protel. > > Has any one else seen this phenomenon? Shouldn't there be a pad everywhere > there is a trace that passes through the board even on in internal signal > layer? > > Thank you for your time and have a nice day. > > > > John Branthoover: > Electrical Design Engineer : > Acutronic R & D:Phone (412) 968-1051 > 137/139 Delta Drive :Fax(412) 963-0519 > Pittsburgh PA 15238 :Email [EMAIL PROTECTED] > USA :WEBhttp://www.acutronic.com > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
