Layer Assignments

[Tom Frayda]

Tom-

I would appreciate it if you would again please list your current layer assignments/usage for the default 30 layers, whether you anticipate changing that structure, and, if so, why. Thank you.


+Tom

[Tom]

Tom,

The below layer plan explains the default 30 layer structure. We use Innoveda's default layer assignments with two exceptions. Layer_20 is used for Placement Courtyards and Layer_19 is used for Gerber Title Block and Alignment Targets.

We used to put a "Board Outline" on Layer_19 also, but recently changed that because of CAM350. Now we have a separate Gerber File just for the real "Board Outline". When you bring a set of Gerber data into CAM350 it's like setting up Layers. You have Copper Layers, Silkscreen Layers, Solder Mask & Paste Mask Layers and now you have a "Board Outline" Layer. The Board Outline Layer is was actually derived from our need to have this in a OBD++ file but we actually like it in Gerber data also. Many people don't know that you can run lots of DRC checks in CAM350 and you can check for entities close to the Board Edge. With the Board Outline being on it's own Layer in CAM350 you can easily turn it on/off. Where as before when we built a board outline into Layer_19 you could not turn it on or off.

Layer & Layer Name
01 Top
02 Layer_2
03 Layer_3
04 Layer_4
05 Layer_5
06 Layer_6
07 Layer_7
08 Layer_8
09 Layer_9
10 Layer_10
11 Layer_11
12 Layer_12
13 Layer_13
14 Layer_14
15 Layer_15
16 Layer_16
17 Layer_17
18 Layer_18
19 Layer_19 Common layer (Below Board Title Block & Alignment Targets)
20 Layer_20 Placement Courtyards
21 Solder Mask Top
22 Paste Mask Bottom
23 Paste Mask Top
24 Drill Drawing
25 CAM Planes
26 Silkscreen Top
27 Assembly Drawing Top
28 Solder Mask Bottom
29 Silkscreen Bottom
30 Assembly Drawing Bottom

[ltrakal]

Tom, there is a document called "The need for predefined layers", I don't know if I have the last version printed of it but the V4.0
Unexpanded Defined Layers is wrong...May be you guys fixed it already and I have an old print?

Laszlo

[Tom]

Laszlo,

Attached is the list of "Predefined Layers for PowerPCB".

This list explains the layer uses and assignments. It also has a new (rearranged) default 30 Layer scheme that makes more sense than the current 30 Layer default.

This document was sent to Innoveda before V4.0 was released. We have not heard a word that they received it or that they are even considering incorporating a logical layer structure into PowerPCB.

[ltrakal]

Oh, ok I'm sorry Tom, I thought that the layer numbering was wrong, but it makes more sense this way than the one that actually comes with the software.

Thanks

[Lameris]

Question:

Why wouldn't you put Silkscreen Top Text, layer 17, on the Silkscreen Top layer, layer 25?

[Tom]

PCBStandards technology follows the same layer scheme that has been used for the past 15 years. Silkscreen Top has always been Layer_26. CADPRO put Title Block Text for "Silkscreen Top" on Layer_17 so that when you post processed an Assembly Drawing you could process Layer_1, Layer_26 and Layer_27. With the new metric library, every part has full padstacks including Layer_27. So now when you process an Assembly Drawing you process Layer_26 and Layer_27. The Title Block text comes out on the Assembly Drawing, but we highly recommend the use of AutoCAD to produce Assembly and Fabrication Drawings. When you bring the Aseembly Drawing into AutoCAD, the first thing you do is delete the Title Block text and then remove the Board Outline under any parts that hang over the Board edge.

Layer_25 has always been used for CAM Planes and every through hole decal in the pcbstandards library has Layer_25 defined in the padstack. When you post process any GND or PWR plane you process Pads & Via's on Layer_25 and a 2D-Line "Board Outline on Layer_25 for the board edge "Plane Pull-in".

Now that PowerPCB V4.0 can process "Custom Thermals", we will switch over to that new process as soon as Innoveda releases V4.0.1 service pack. There are many users who are still on V3.5.1 and V3.6. The pcbstandards through hole library parts have "Custom Thermals" already defined and ready to go.

[sethg]

Hi Tom - I noticed in your 30-layer scheme that you mentioned you have gone to a separate layer for board outlines but did not indicate which layer that is. Is this something you're still experimenting with or are you convinced it is the better way to do things? If so, would you care to update your 30-layer list and show the board outline layer. BTW, I like the arrangement you show in your V4 layer usage, both the expanded and unexpanded. They are both much more logical than the stock PowerPCB layer definitions.:) It's almost embarrassing how much time I spend searching for silk top and silk bottom, etc., even though I've done it a thousand times before. Having them in a logical order is long overdue.

How do we pressure PADS into adopting your proposal, or any standardization for the expanded layer set, for that matter? :confused:

[Tom]

Seth,

"Board Outline" is on Layer_0 (All Layers). In File/Cam there is a separate button to post process "Board Outline". What we did, in the new 2002 Start and CAM files was to add a text string on Layer_25 called "Board Outline (Top View)" in the Title Box. Layer_25 was selected for this text string because we have never processed "Text" on Layer_25 for any other purpose.

It became really obvious to us when we started using CAM350 a lot that processing a separate Gerber File for "Board Outline" had great advantages. Designers who do not use CAM350 are unaware that when you import Gerber data into it that it creates a Layer for each file. The CAM350 user can turn on and off layers to perform certain DRC checks and use the Board Outline layer for NC Route data. Basically it gives the CAM operator greater flexability.

I too after using PADS software for many years still have trouble remembering what layer is "Bottom Silkscreen" and it is not getting any easier the older I get. A logical layer assignment is way past due and really should have been done in PowerPCB V1.0, but there must be some kind of a major hassle to incorporate this change. It's always easy to say "Here's a great idea for a new feature", but implementing a new feature or revising an existing feature sometimes impacts the software so deep that the change requires too many man hours to maintain profitability.

A good example of a simple change is this "Board Outline" as a separate Gerber file. We had to edit 120 CAM Files and 120 Start Files (2 - 16 layers), which took a week (at Wind Rivers expense) just to add this simple feature.

Regarding "How do we add pressure?" to Innoveda to adopt a standardized layer scheme is beyond me. PowerPCB features are put in two categories "Bugs with Tracking Numbers" and "Wish List". This is definitely a "Wish List" item and that would fall into the User Group "Advisory Board" and Josh Moore (PowerPCB product definition manager). You can find all the names and e-mail addresses of every member of the Advisory Board here http://ug.innoveda.com/advisory_board.htm

[ltrakal]

Tom, where is that button you talk about? "In File/Cam there is a separate button to post process "Board Outline". "....and why the gerber output settings are in inches? i'm finishing my first board now and ready to send gerbers but the PCB house ask me for 274X not 274D...isn't that the standard one? why is in the library the 274D checked? should I change the units to metric?

Thanks
Laszlo

[Tom]

The Gerber Output Settings are a "System Parameter" which needs to be set to "Metric" by you. Once you set it, it will stay that way until you reset it. I.E.: Setting Gerber Output Units to Inches, Mils or Metric does not stay with the PCB design, it is a "System Parameter".

The "Board Outline" check box is in File/CAM/Edit/Layers.

The 274X has the apertures defined in the Gerber data. This is also a "System Parameter" and must be set by the User. Once you set it, it will stay that way until you reset it. This means that every design you post process will be processed using 274X.

What you are experiencing is a new software install. Everytime you install PowerPCB, you have to go to the File/CAM/Edit/Device Setup/Advanced and setup your parameters. Then they will always stay that way until you load a new revision of PowerPCB or you manually change them. These settings do not stay with the PCB design, they are "System Parameters".

Your advanced settings should be:
Units: Metric
Number of Digits: 3 / 5
Coordinates: Absolute
Zero Suppress: Leading
Output Format: RS-274X

[ltrakal]

Tom, I have to take hat off whenever I see you.

Thanks a lot

[davepcb]

I am confused. I read several threads about board outline. Do I create a board outline in the "all layers" then go to layer 25 and draw a 2D-line for plane pull in?

I checked out one of the board outline's from the site index and saw that it was on layer19. Can I change that to all layers some how? I'm trying to follow everything in pcbstandards.

davepcb

[randychase]

The board outline should be on all layers. A 2D line in V34 4 can be converted to a board outline and changed to all layers by selecting the entire line (shift-click), right mousebutton, and select SCALE. Use a scale of and change the item to board outline.


The negative clearance for a neg cam plane should be on L25. Simply copy the board outline and do the same thing above. Change the copy to 2D lines and to Layer 25. Then change it to a much fatter width.

[Tom]

The Board Outline is the only element that is inserted on "All Layers". This is necessary because the autorouters obey it's presence on all the routing layers. When you create a Drill drawing or an assembly drawing you should use Board Outline. (Note: We make the Board Outline Width 0.5mm)

The Board Outline is built into every CAM File as the first photoplot. For years we processed the Board Outline on every Gerber file but we learned from our manufacturers that they prefer having one Gerber file that is the Board Outline so that they can turn it on and off as they wish. They can also use the Board Outline Gerber data as NC Route data.

The post-processing units are configured at the system level. They are not something that you can program into a CAM file. Every time you install a PowerPCB Patch or Upgrade it resets your post processing units back to Inches. This needs to be addressed by Innoveda (Mentor). They need to change the installation process so that the user can select the correct units that they are working with at the software installation level.

It drives me crazy to have everything defined in metric and then do a PowerPCB install and have all the defaults changed back to Inches.