Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Altium designer error message

Status
Not open for further replies.

krunal_299

Member level 4
Joined
Jan 24, 2008
Messages
68
Helped
2
Reputation
4
Reaction score
1
Trophy points
1,288
Activity points
1,800
the film is too small for this pcb

Hi to ALL!
i am using altium designer for PCB development.
When ever I am trying to generate Gerber files as output, the following message is prompted:
"The film is too small for this PCB "

I dont counter where the problem is.
Pls let me have some solution on it.
Thanks & regards!
 

error altium designer

You either have a stray object that is far away from your PCB, or you just need to increase the film size in the Geber setup dialog.

What happens if you hit the shorcut keys VF (View>Fit Board) while in the PCB Editor? Your display should zoom in and display only the PCB. If it shows the PCB as a smaller image in one of the corners of the screen, then you have some stray object that has been accidentally moved or placed outside of the PCB. This sometimes accidentally happens because you move something you didn't intend to move. You can sometimes delete the stray object by using SA (Select All), then using XI (deselect inside) and drawning a box around your reall PCB and notes, then using delete to get rid of the stray object. If that doesn't work, you can use the PCB list panel, sort by x,y coordinates, and locate the object that is far away from the others on your board. You can then move in closer and modify or delete it. Sometimes it's just a stray comment field for a component, and you just need to move it in close and hide it.

If the problem is just small film size, go File>Fabrication Outputs>Gerber Files. On the "Advanced" tab of the setup dialog, you can adjust the film size. If you are using an OutJob to generate your files, you can get to the same dialog from the OutJob Gerber line by double clicking on the line. The film size setting is a leftover from the days of older film plotters, and doesn't affect the quality of your Gerbers. It was once used to make sure that your plot would fit the standard films available to fabrication plotters. The new CAM equipment today at the fab takes care of positioning and film sizing.
 

film is too small for this pcb

Thank you very much!
Got solved.
but new problem i am facing :
In schematic design when i am trying to compile the project, the following message appears as warning:
"Unique identifier errors"
Which leads to misbehaviour during schematic to PCB board transfer.
Even the designators are same in PCB and Schematic , the ECO promts every time to resolve the difference.
So ultimately there is no communication link for the components between PCB and Scematic.

I knew that this message is related to components unique ID generated by system itself.
But dont know how to reset these component IDs in scematic to disappear this warning message.
Regards!
 

altium designer errors

To synchronize your component ID's between the PCB and schematic, open the PCB document for your project. Now go to the menu item 'Project>Component Links' in the PCB Editor. Once you click on that, the dialog will lead you through the process of matching component designators to get the ID's matched up between the schematic and the PCB. You may have to repeat the process a couple of times to get it all straightened out - it depends on how messed up things have gotten.

The same menu choice 'Project>Component Links' is available from the Schematic Editor if the problem is on the schematic side.

If the compiler is reporting the error only for the schematic, then you have duplicate ID's for some components. You can fix that by looking at which components are being reported in the "Messages" Panel. You can then double click on the schematic symbol for one of the components, and choose "Reset" Unique ID from near the top left of the dialog. Then recompile, and use the 'Component Links' menu to fix the match between schematic and PCB.
 

unique identifiers error altium

Thanks !
I will let u know after trying this one.
I think you are versed player for Altium designer.
That's great!
Can you suggest me any source or example project which demostrates the autorouting feture for PCB editor(i.e. learning Effective use of Autorouting during design process)?

Regards from bottom of the heart.
Bye..
 

the film is too small for the pcb

Hi again House cat!
Can u pls tell me how to reset the unique id of all the components in schematic at once?
The same menu choice 'Project>Component Links' is available from the Schematic Editor if the problem is on the schematic side.

This option does not get highlighted (i.e. not activated ) in schematic editor.
regards!
 

error film too small in altium

Aside from the documents in the Help directory of your Altium installation, there aren't any tutorials on the use of the Situs Autorouter. I have attached a short note with some suggestions on setups that give good results.

The Component Links menu selection in the Schematic Editor no longer works. Altium will probably remove it from the menu in a future update. They have used unique ID's for schematic parameters, directives, snippets, and now Design Sheets. They don't want you to be able to reset all of those unique ID's from the schematic editor. They want you only to adjust unique ID's from the PCB to match components. If you need to reset a unique ID for a symbol on the schematic, you can do it one-at-a-time by double clicking on the symbol. The properties dialog will let you reset the ID for the symbol. You can then compile the schematic, and go to the PCB to resynchronize the ID with the PCB component.
 

ad6 the film is too small for this pcb

Thanks a lot!
I am downloading the link provided by you.
And about unique ID reset, my question is about reseting unique IDs of all the component at same time at single operation.
You are suggestin for single component(1 by 1.)
Thanks & regards!
 

altium snippets

You cannot reset all of the unique ID's with a single operation. As I said above, AD now uses unique ID's for more than just the components.

You can reset the designators all at once from 'Tools>Reset Schematic Designators'. You then use either 'Tools>Annotate' or 'Tools>Force Annotate All Schematics' to reassign new designators. If you already have a PCB, and you reset the designators for the schematic, you'll have to resynchronize the board with the schematic by compiling and sending the information to the PCB.
 

An extra tip: The rooms can also effect the film size. Try doing the Wrap Rectangular Room around components for all the rooms on the board
 

Re: the film is too small for this pcb

This happened to us because some components got placed off the board (e.g. at -44000 mils). We don't know how this happened, but none of the suggested techniques like "view | Fit Document" would locate them onscreen.

Our solution was to use Shift-F12, as per this **broken link removed**, to see the list of everything. By editing the coordinates in this list, we were able to move the offending parts onto the visible and accessible (positive x, y) portion of of the board, then delete them as usual. Hint - clicking on the column headings at the top will sort the list on that column.


Hi to ALL!
i am using altium designer for PCB development.
When ever I am trying to generate Gerber files as output, the following message is prompted:
"The film is too small for this PCB "

I dont counter where the problem is.
Pls let me have some solution on it.
Thanks & regards!
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top