How to make copper pour on a layer if PCB Editor crashes every time I try to place a shape?

Not really enough information. What version are you currently running ?.

Is your licensing running locally on your pc or is it on a networked server ?

When you ran dbdoctor check did it report any errors with the database ?

I am curious about this since I have used Allegro/Orcad pcb editor for a long time and have never seen it crash. In particular shapes would be one of it's strongest points "Copper Pours" etc.

Let us know and maybe we can help you out.

Thanks ...

Thanks for the reply.

I am running 17.4-2019 S006 [4/21/2020] Windows SPB 64-bit Edition, OrCAD PCB Designer Standard.

It's a node linked license (server running on my PC)

The doctor prints:

Checking db records

checking for orphans...

Checked 35 percent

Checked 71 percent

Loaded existing device file 'C:\Users\[..]\Documents\ORCAD\[.]\Layout\devices.dml'

Finished loading SigNoise device libraries

Checked 100 percent

Done dbdoctor.

I can only envy your positive experience, because I use ORCAD for one month and it keeps crashing whenever I try to place a shape on any etch layer.

I am still trying to troubleshoot the problem. Here some of my observations:

- I followed EMA tutorial for copper pour - works fine

- My design uses multiple part models from Digikey, Mouser and others placed on a circular board with a rectangular cutout about 25% of circle area. The cutout extrudes off the circle, i.e.the board  looks like a round waffle after a bite :)

- If I import my netlist to a rectangular PCB I can add pour with no problem

- If I use netlist from the tutorial on my circular board outline, the pour fails, that looks like I have a problem caused by complex shape of the board outline

I have quite a limited time for the design, so I had to move on without flooding my layers with copper at least for the first prototype. 

Thank you very much for the analysis. Unfortunately I am not that advanced in Orcad to use your suggestions without more detailed description. The way I created the board outline was the simplest possible: DesignWorkflow->BoardOutline->Create, I just drawn a circle and a rectangle than spent 20 minutes to find how to convert them to cutout. Then I used Place->Mechanical symbols to add 6 holes and after this never touched outline at all. If I understood you right I will need to add ute Keepin all and Package Keepin ? I'll search youtube tutorials on how to do this, or if you can provide some brief step-by-step guidance, please help.

I also upgraded to hotfix 7 which really gave me a small improvement, once I was able to make a pour that overlaps the cutout, however the program is still very unstable and crashes with no diagnostic  if I try to place a shape on "etch" on any layer. This is a serious bug itself, loos like an uncaptured event, a 30 years old software should not behave this way.

Hi, I honestly think there is something wrong with your install of the software. I have all versions here including the latest 17.4 which I don't use as much as 17.2 or 16 x and have never seen the software just plain crash like you are describing. Certainly all software can and will have bugs but I have found the Orcad/Allegro pcb editor very robust.

FYI, when you install Allegro there are a few install options and one with pitfalls. On a windows system my advice is to install the software for "All Users" and not the current user. You will know if you had installed for all users because under you C:\ drive or the drive you installed to you will see a folder c:\SPB_Data, This particular folder contains the variable settings for both Capture and also the PCB editor.

On the board outlines and keepouts, I imagine It is fine to use the design workflo, I have never used it but if you want to do that manually here is how.

1 "Create a circular board outline"

Click on shape & choose circular, next go to the visibility tab and select "Board Geometry" and choose the subclass of "Design_Outline" - On the canvas draw your outline to the size you want and double click the left mouse button to complete.

2 "Create a route keepin-all layers"

The same as above but this time we want to create that circular shape on the "Route Keepin" ALL class subclass.
Click on shape & choose circular, next go to the visibility tab and select "Route Keepin" and choose the subclass of "All" - On the canvas draw your keepin to the size you want and double click the left mouse button to complete. Note: typically a keepin is backed off anywhere from 50 to 100mil from the edge of the board.

3 "Create a Package Keepin"

Same procedure as above but this time choose "Package Keepin" with a subclass of all. You could make this the same size as your board outline or smaller. Basically this is used by drc to determine how close a package "Footprint" should be to the edge of the board.

Now that you have created that board outline manually with the keepin's etc try add a shape to the board. In the visibility tab choose "Etch" and select the etch layer you want say the top layer.
Click on Shape choose Rectangular and draw a big rectangle over your board outline. You should see that the actual shape only fills the inside of the board. The reason the shape only fills the inside of the outline is because you have a "Route Keepin" and since that keepin is on all layers the shape wont extend beyond the board outline on any etch layer. Cool eh :).

There are other ways of doing this too beyond simple rectangular boards or circular similar to the example I described earlier. Hopefully this info will help you out.

All the best.

This is what happens when I follow the instruction:

1. Board outline is basically the same, I just reproduced the same shape

2. Route Keepin is trickier, because to create a cutout I place a circle first:

But when I try to place a rectangle (to merge them into a cutout), the circle disappears:

It looks like poligone could work, but to build a circle with cutout of poligones is not realistic.

I tried to continue with simple circular keepin. It allows to add a pour to one layer(with cutout also flooded), but crashes when I try to do the same on another layer.

Try using Shape - ZCopy, look at the Options pane and set the class/subclass to Route Keepin/All contract to say 0.5mm and then left click the design outline. This is like an offset command that copies the outline to the keepin but 0.5mm smaller. Much easier than re-drawing. 

Well maybe a different approach will get you to where you need to be. When it comes to creating more complex geometry Allegro is certainly up to the task but the first thing and the easier road to go is to actually draw what you want. For the moment don't worry about keepouts or board outlines or any of that stuff. The key is how to draw the actual geometry of what you want.

So how to do that.

With a fresh board go to "Add a Line" on the tool bar and draw the top part of your cut out to be that size. Down in the bottom of the screen you will see the coordinates displayed, cycle to R mode which is relative so you can see how far you had drawn the line. You can place the line on the following Class Subclass - "Board Geometry - Silkscreen top", In the picture below those lines are 1200 Mil which is close to 30.4 mm. (Still use Imperial units in the USA)

Ok the next part is how to draw the circle so to do that we go to the tool bar and choose "Add - 3PT ARC" In the picture above Left click on top the upper right side line and draw a line left. When you get to the top left line, left click then drag the mouse down. You will see the circle start to appear. Drag down until you reach the desired size of your circle. From your earlier picture I made the circle in the pic below to be 3000Mil or 66mm.

So with this basic geometry you have a great starting point. From here you will have to figure out how to get that geometry converted to be a board outline and keepout etc. That part is not that hard really. Maybe you can figure it out but if not I can show you how.

BTW if Orcad is still crashing on you, You should call support. It is plausible that your whole design could well be corrupt.

All the best.

Well maybe a different approach will get you to where you need to be. When it comes to creating more complex geometry Allegro is certainly up to the task but the first thing and the easier road to go is to actually draw what you want. For the moment don't worry about keepouts or board outlines or any of that stuff. The key is how to draw the actual geometry of what you want.

So how to do that.

With a fresh board go to "Add a Line" on the tool bar and draw the top part of your cut out to be that size. Down in the bottom of the screen you will see the coordinates displayed, cycle to R mode which is relative so you can see how far you had drawn the line. You can place the line on the following Class Subclass - "Board Geometry - Silkscreen top", In the picture below those lines are 1200 Mil which is close to 30.4 mm. (Still use Imperial units in the USA)

Ok the next part is how to draw the circle so to do that we go to the tool bar and choose "Add - 3PT ARC" In the picture above Left click on top the upper right side line and draw a line left. When you get to the top left line, left click then drag the mouse down. You will see the circle start to appear. Drag down until you reach the desired size of your circle. From your earlier picture I made the circle in the pic below to be 3000Mil or 66mm.

So with this basic geometry you have a great starting point. From here you will have to figure out how to get that geometry converted to be a board outline and keepout etc. That part is not that hard really. Maybe you can figure it out but if not I can show you how.

BTW if Orcad is still crashing on you, You should call support. It is plausible that your whole design could well be corrupt.

All the best.

Thanks, I just typed a reply that was lost somehow. I followed the instruction, however there is one small detail I cannot fix: after I drawn the shape on the silkscreen it appears to be a set of separate shapes, even though I entered all point values manually, i.e. en of one line is explicitly set to be start of the next one and same for the arc. Is there a way to combine them into a single shape to avoid message "Not a closed polygon"?

Ok then we are down to the last part. Getting there eh :)

So a couple of things. You are correct in that if you draw lines etc that the geometry will not be closed but this is ok because we will use this geometry to create what we need. In Allegro shapes are really powerful more so than any other PCB tool I have seen. Basically you can make shapes directly or indirectly using lines as the basis.

So to refresh we have the geometry we need and we put this geometry on a layer that is the "Board Geometry - Silkscreen Top", we could have put it on another layer too. The idea is just to get what we needed drawn first.

Here is what we have again for clarity just to refresh.

Next we want to convert this geometry to a "Board Outline" & also a package keep in & a route keep in.

In your find filter make sure both Lines & shapes are checked.

1 Go to the tool bar and choose the shapes menu and select "Compose a Shape"  - On the right hand side options panel you should see something similar to the pic. Notice that the options default to etch which is ok as we will change the options to suit.

Here is a pic:

Change the options to:

Active Class "Board Geometry" - Add shape to sub class Outline, I'm using 16.6 so I use outline which is the board outline. In 17.4 you would choose Design Outline I believe.

Another Pic:

Lastly with your mouse left click and hold the left mouse button down on the canvas and draw a box to encompass the geometry. The geometry will highlight, Right click and select done.

You now have created your "Board Outline"

Here is another pic of the completed Board Outline.

So that's very cool & when you get used to the mechanics of things you can see the potential this actually has for creating very complex shapes or board outlines etc. Lots of possibilities exist .
In Allegro you can Compose shapes from lines & also decompose shapes to lines.

Ok then down to the final bits. You still have to create your Route Keepin & also your package keepin. I f you turn off the Board Outline layer in the options panel you will see you still have your original geometry on the board outline silkscreen top layer so you can re-use this original geometry to make the additional Route Keepins and Package keepins you need by doing the same process again.

When you create the additional items they will be the exact same size as the original geometry. When you get the last items made a good rule of thumb is to back them off from the board outline by say 50 Mil OR 100 Mil, this will be easy to do as Allegro gives you the ability to Shrink or expand shapes.

Basically what you do is select the shape - say Route Keepin all and right click and choose Expand/Contract, reduce the shape by the amount you need using the buttons in the options panel.

Here is a pic showing the route keepin reduced by 100 mils.

After all is complete you can delete your original geometry from the Board Geometry - Silkscreen top layer.

BTW there is another way to do this that kind of speeds up the operation too.

All the best

The support suggested a workaround for this bug. The problem disappears if Design accuracy is set 2 and it really worked.