At 10:01 AM 1/8/2004, Tim Fifield wrote:
One problem I've encountered is as follows; this was taken from Protel
Knowledge base:
Query: Why do I get an error message: "The Film is too small for this PCB"
when I generate Gerber files?

Answer: This occurs in two cases. Either the Gerber film size is smaller
than the PCB, or the PCB file contains off-board objects that make the
extents larger than expected.

Mr. Fifield then says that the procedures given don't fix the problem. But we need more information.

This problem is basically the same with 99SE. Actually, there is only one case, which is that there are objects outside the plottable film area. In the first situation, the film is simply too small, and in the second, there are objects outside the workspace (or perhaps in the workspace but outside the film and perhaps invisible under most circumstances.)

To enlarge the film size in the Gerber setup dialog [I'll skip this, it is straightforward, but remember the film size should preferably include a 1 inch border all around.]

If these values
already seem large enough for your PCB, return to the PCB editor and press
Ctrl + Page Down (or select View > Fit Document). If your PCB file contains
objects outside of the board's edges, the screen will resize to contain
these objects (if they're very far away, the board will appear very small).

Did this happen? I.e., did the board as determined by this operation (Zoom All, Z-A is a fast way to do it) seem to be larger than you were expecting. Did it continue to be this way?

To clean up the extra primitives, deselect everything by pressing XA (Edit >
Deselect > All), then press SO (Edit > Select > Outside Area) and drag
around the whole board.

I expect this, however, will fail if the object spans the board and extends outside the workspace. It may be better to Select All and Deselect Inside. Objects which are inside and extend outside will then remain selected, as I recall.

Before deleting, you may open the List panel (F12) and review the selected
objects (right-click for an option to remove non-selected objects from the
list). Once these objects are deleted, or otherwise returned to their
rightful place within the extents of the PCB, the film error should be

My problem is that we did all this and it still gives me this error. I tried
selecting board and moving it to a new PCB page and I tried selecting the
PCB inside area and moving it to a new pcb page as well. Nothing seem to

Not enough information, yet. Are you seeing symptoms of extraneous primitives (other than the film size problem)? If so, you need to delete them. It should not be necessary to copy the whole thing elsewhere; if somehow you manage to select a spanning object, it will also be in the copy. For example, a component may have a wayward primitive, such as a .TYPE string, sitting in negative space. I've just verified, by the way, that DXP is like 99SE in allowing primitives to exist outside the workspace. You can create these by moving a selection. Your reference point must remain inside the workspace, but some of the moved primitives might end up outside the space.

What do you see when you do Zoom All? If you select a few objects and pick them up and wave them about rapidly enough, Protel abandons redrawing the objects and instead draws a bounding box. If you have selected everything and then deselected inside, suppposedly deselecting everything in your design, the bounding box described should only enclose the few test primitives you just created, selected, and are moving. If it is bigger than that, you can get an idea where the offending primitive is, because the box will have extended as necessary to include it.

In 99SE I would, under these conditions, move the offending primitives into the workspace.

In DXP, the command to zoom to a view that includes all primitives is Zoom All (Z-A).

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * * * Browse or Search previous postings: *[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to