AnsweredAssumed Answered

Xpedition FabLink Drawing Editor manufacturing outline

Question asked by stempialdo on Feb 1, 2019
Latest reply on Feb 14, 2019 by greghall

Like • Show 0 Likes0
Comment • 12

Hi there,

If I try to import a board into the FabLink Drawing editor I get an error saying "The board outline of the design, is not completely inside the manufacturing outline".

This is not actually the case as in Layout (VX.2.4) the manufacturing outline matches the board outline (or I get the same error even if I have extended the manufacturing outline as far as possible, way bigger than anything else in the design).

As a result, the board import into the Drawing Editor is not really successful; it only imports the board outline without any parts, tracks or plane (all layers visibility enabled).

In fact the component explorer only contains the drawing cell and the board outline. That means I can't create the assembly drawing etc..

Does anybody know what I am doing wrong?

cheers

Flavio

stempialdo Feb 14, 2019 7:57 AM

Correct Answer

For future reference, if anyone has the same "sync" problem between the PCB and Fablink Editor:

the problem happens if you click "Cancel" in this warning after the import (and also if you tick the box..).

So it was my bad!

Hope this helps

Flavio

See the reply in context

No one else had this question

Outcomes

12 Replies

Jackie_D Feb 1, 2019 6:19 AM
Mark Correct
Correct Answer
Hi Flavio

Several thoughts about this:
Are there Variants defined for the PCB? If yes, the FL Variant Data must be generated before trying to import the board into Drawing Editor.

Even text or something on a User layer that crosses the manufacturing outline will cause the message, so try turning on User Layers as well in Display Control. It may also be worth doing ECO > Reset Cell to ensure that there is no cell placed near the edge where the graphics have been deleted but the cell origin is still placed.

If this doesn't help, open a Service Request and we'll take a look at it.

Regards
Jackie
Like • Show 0 Likes0
Actions
stempialdo @ Jackie_D on Feb 4, 2019 2:34 AM
Mark Correct
Correct Answer
Hi Jackie,

thanks for your reply.
No, there are no variants defined for this PCB.
Everything is enabled "loc: All on", plus all the User Draft layers. No luck with resetting the cells.
The manufacturing outline is a big rectangle bigger than anything else but I am still getting the error message. Ok I will raise a Service Request.

Do you know how to completely remove a cell from the design (with the origin included)?
If for example I wanted to remove the Fab_Notes that I find the PCB template, even after removing the cell instance from the design in the Cell Editor I cannot delete the cell from the local library (I get the error message "This cell cannot be deleted because it is referenced in the design").
Is there a special way to delete the instance of the cell so that I can be deleted in the cell editor?

Thanks
Flavio
Like • Show 0 Likes0
Actions
Jackie_D @ stempialdo on Feb 4, 2019 2:48 AM
Mark Correct
Correct Answer
Hi Flavio,

Even a Drawing Cell must be deleted in Place mode to remove it completely from the design.
Deleting only the graphics of a drawing cell in Draw mode will leave the Cell Origin and reference to the cell. In this situation it is possible to run ECO - Reset Cell and get the whole cell back in the design.

Regards
Jackie
1 person found this helpful
Like • Show 1 Like1
Actions
stempialdo @ Jackie_D on Feb 5, 2019 7:06 AM
Mark Correct
Correct Answer
Hi Jackie,

thanks for your reply. Yes, deleting graphics in place mode works! Thank you for the tip.
I guess I need to be very careful not to delete items while in Graphics mode (otherwise if I do, then the graphic instance disappears and then I am doomed with no way to completely delete the cell).

Also .--.. thanks for pointing out to the script; it works very well. Seems a bit of an overly complicated way to delete stuff but, given the above, I now understand why somebody went through the exercise of writing that script. Very useful!

Now there is nothing outside the manufacturing outline, as you suspected I had an "hidden" item outside (text with 0 height far away from the center). But the board import still gives that error.

Anyway thank you for your help!

Flavio
Like • Show 0 Likes0
Actions
Jackie_D @ stempialdo on Feb 5, 2019 8:04 AM
Mark Correct
Correct Answer
Hi Flavio

Even if you delete items in Draw mode from a drawing cell so it is not possible to see where it is placed, you can still use ECO > Reset Cell and select the appropriate drawing cell name to have it refreshed from the local library onto the design and thus available for deleting in Place mode.

The InsideOutside script is great for finding items that have wandered off for whatever reason :-)

Regards
Jackie
Like • Show 1 Like1
Actions
stempialdo @ Jackie_D on Feb 5, 2019 8:34 AM
Mark Correct
Correct Answer
Thanks Jackie
Like • Show 0 Likes0
Actions
.-.--.-- Feb 4, 2019 6:20 AM
Mark Correct
Correct Answer
Flavio,

In Xpedition, try running the script found at this link: Expedition/Cell Editor: What's Inside/Outside? It may help identify objects outside of the manufacturing outline.
1 person found this helpful
Like • Show 0 Likes0
Actions
caleigh_gold Feb 6, 2019 10:01 AM
Mark Correct
Correct Answer
stempialdo I hope you found this discussion useful! Has your question been answered?
Like • Show 0 Likes0
Actions
stempialdo @ caleigh_gold on Feb 6, 2019 10:19 AM
Mark Correct
Correct Answer
Well it is useful to know how to spot a "rogue" graphic item in the design, but the original problem is still there as I keep getting the import error.
But I guess that problem is more for a service request rather than the form.

But thanks for the assistance, I received good support!

cheers
Flavio
Like • Show 0 Likes0
Actions
stempialdo @ stempialdo on Feb 13, 2019 8:23 AM
Mark Correct
Correct Answer
Hi there,

I think I have found the root cause of my issue:
basically even if I change the manufacturing outline to something huge (and I remove anything outside it with that handy user script), I still get the error above.
However, I have now realized that the issue is that the import is not using an updated version of the PCB. In fact, even if I move IC's around or even change the PCB board outline, when I import the PCB into the Drawing editor I still see the "original" version of the PCB.

That is strange because in the Drawing Editor manual it says:
Any modifications to one drawing file do not reflect in other drawing files; however, any
changes to a board/panel design dynamically update all drawing files that include that design.

This is clearly not working for me (that's why changing the Manufacturing Outline in the PCB had no effect).

Any clues? What am I doing wrong?

thanks
Flavio
Like • Show 0 Likes0
Actions
stempialdo @ stempialdo on Feb 14, 2019 7:57 AM
Unmark Correct
Correct Answer
For future reference, if anyone has the same "sync" problem between the PCB and Fablink Editor:
the problem happens if you click "Cancel" in this warning after the import (and also if you tick the box..).

So it was my bad!

Hope this helps
Flavio
Like • Show 0 Likes0
Actions
greghall Feb 14, 2019 8:04 AM
Mark Correct
Correct Answer
Think actually the answer to your original question about the parts not being displayed.
Is that after opening Fablink, need to select Place -> Upload All Design Data
Then all components and tracks will be displayed on the panel.
Like • Show 0 Likes0
Actions

Xpedition FabLink Drawing Editor manufacturing outline

Outcomes

Related Content

Recommended Content