Altium Designer/Protel - 'Film is too small for this PCB' error

Includes information regarding protoyping, technical questions, company news, and input about our products.

Moderator: Sunstone Moderators



Altium Designer/Protel - 'Film is too small for this PCB' er

Postby Terri Miller » Mon May 14, 2012 9:30 am

I ran across further information on other objects that may cause this error and a possible solution in resolving the issue: There can be several issues when you get the error in Protel, Film too Small for PCB; Usually objects outside the board area. Most objects can be deleted easily because they are visible. Phantom Polygons are not visible so the steps in deleting them differ than only selecting and deleting outside objects. Here are instructions to resolving the issue.

Detecting/Removing Phantom Polygons:
To detect invisible, "phantom", polygons, check how many polygons there are visible on the PCB and compare it to the number of polygons reported in the Reports Board Information dialog. If the comparison does not match, where Board information reports more polygons than there are actually visible, then it's most likely that "phantom" polygons exist and the PCB needs to be cleaned up to avoid problems.

A method to clean up the PCB:(Note: This procedure will remove all polygons unless specific polygons are chosen in step 7. "Phantom" polygons usually have a point count (vertex) of 1 or less. See the Point Count column in the spreadsheet in step 7.)

1. Turn on an arbitrary signal layer that is not used. Select Design Options Layers TAB dialog and enable a signal layer, e.g. Mid Layer 1.
2. Place a polygon on the enabled layer.
3. Choose Edit Deselect All.
4. Choose Edit Export to Spread.
5. The wizard will pop up. Press Next and then uncheck all the options except for Polygon. Proceed to complete the wizard.
6. Once the spread has been created, go to the Layer column in the Spreadsheet.
7. Set the layer attribute for each polygon to the arbitrary layer.
To remove a specific polygon change the layer attribute to the arbitrary signal layer and leave the rest the same. When changing all or a range of cells, click on the cell to copy, use copy then click and drag on the cells to be changed and then use paste. Copy and paste can be found on the Edit menu or on the right mouse click menu.
8. Select File Update and this will update the PCB file. (Make sure that the spread is closed after the editing session because if this procedure is repeated it will open another spread document and FileUpdate will not work. Only 1 spread document can be open at a time for the Update process to work.)
9. Click on the arbitrary layer TAB in the PCB window, Mid 1 in this case, and choose Edit Select All on Layer (shortcut s,y).
10. Choose EditClear (shortcut CTL+Del).

This should remove the polygons which could not be seen or edited. Check the Board Information report to see if the required polygons have been removed. ~ Terri
Regards,

Terri Miller
Sunstone Circuits
13626 S. Freeman Road
Mulino, OR 97042
Phone: 800-228-8198
Fax: 503-829-6657
Terri Miller
 
Posts: 38
Joined: Thu Sep 01, 2011 12:00 am

Re:Altium Designer/Protel - 'Film is too small for this PCB'

Postby Terri Miller » Mon May 14, 2012 9:30 am

Hello,

Using Altium Designer/Protel software, you may have seen this error: "The Film is too small for this PCB." This error will occur if the Gerber film size entered is smaller than the PCB or the PCB file contains off-board objects that make the extents larger than expected.

To enlarge the film size: Select File > Fabrication Outputs > Gerber Files; Go to Advanced tab and enter appropriate X & Y values for the film size. To clean up off-board objects: Deselect everything by choosing Edit Deselect All. Go back to Edit > Select Outside Area and drag around the entire board. Delete & save. *Note: Always closely review objects selected before deleting!

I hope this information helps!

Terri
Regards,

Terri Miller
Sunstone Circuits
13626 S. Freeman Road
Mulino, OR 97042
Phone: 800-228-8198
Fax: 503-829-6657
Terri Miller
 
Posts: 38
Joined: Thu Sep 01, 2011 12:00 am

Re: Altium Designer/Protel - 'Film is too small for this PCB

Postby waleeedijaz » Wed Mar 02, 2016 1:00 am

Using Altium Designer/Protel software, you may have seen this error: "The Film is too small for this PCB." This error will occur if the Gerber film size entered is smaller than the PCB or the PCB file contains off-board objects that make the extents larger than expected.
waleeed
waleeedijaz
 
Posts: 1
Joined: Wed Mar 02, 2016 12:57 am

Re: Altium Designer/Protel - 'Film is too small for this PCB

Postby Robert Ohanesian » Wed Mar 02, 2016 5:26 pm

Thank you for your assistance. Hopefully everyone that uses Altium is able to benefit from that information. If you have any further questions I would recommend that you send them to support@sunstone.com.
Regards,

Robert Ohanesian
Customer Support
Sunstone Circuits
13626 S. Freeman Road
Mulino, OR 97042
Phone: 800-228-8198
Fax: 503-829-6657
Robert Ohanesian
 
Posts: 49
Joined: Thu Oct 16, 2014 10:18 am




Return to Products and Services

Who is online

Users browsing this forum: No registered users and 2 guests