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.

Importing .dxf file in Allegro

Status
Not open for further replies.

HANUMAGOUDA

Member level 1
Joined
May 17, 2010
Messages
40
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,288
Location
BANGALORE
Activity points
1,550
Hi Experts,
I am facing one problem while importing .dxf file in allegro. whenever i am trying to import the .dxf file i am getting only the outline(template outline), even though it contains texts .
what i need to do to import the .dxf file without any problem. So can any experts tell me the procedure to import .dxf file.
step by step procedure is very helpful. Please do help me.

Thanking you.
Hanumagouda Patil
 

ckshivaram

Advanced Member level 5
Joined
Apr 21, 2008
Messages
5,070
Helped
2,149
Reputation
4,304
Reaction score
2,089
Trophy points
1,393
Location
villingen (Germany) / Bangalore
Activity points
30,086
you're using Allegro is to open it with IntelliCAD (it comes with newer versions of Allegro. look in the install folder structure. it's there for installing), and then save it as a version 14 or earlier .dxf file.

or

For importing DXF go to file import DXF select your DXF file preferably in Allegro folder. If you have already defined your layers select Incremental addition, failing to do so results in lost of all your layers. Also you need to know which unit your DXF was created select it accordingly. Now you need to create conversion file click on tab to browse and type a name for your file click open. Then go to Edit/View layers here you have to map DXF layers to Allegro after mapping the layers click ok then import.

If you follow the above steps then you will see how to edit CF in dialog box of DXF import. The file name can be given by user or you can use Allegro assigned name.
 

HANUMAGOUDA

Member level 1
Joined
May 17, 2010
Messages
40
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,288
Location
BANGALORE
Activity points
1,550
Thanks for your reply shivram,
I followed your steps but still i am not getting the text inside the template. i am using Cadence V16.3 for my design.
I am not getting Intellicad software in my installed directory, can you please tell me the default location of this software?
In the mean while can you plz tell me little bit clearly how to import .dxf file with texts.

Regards,
Hanumagouda Patil
 

Uky

Member level 5
Joined
Sep 3, 2004
Messages
83
Helped
18
Reputation
36
Reaction score
4
Trophy points
1,288
Location
Swedish West Coast
Activity points
1,205
What you need is to have some drawing editor that can access the .DXF-file. It is often the case that the drawing needs to be edited/repaired.
For instance: The board outline should ideally be a closed polyline. You also need to know the name of the layers and what they should represent
in the imported design. An editor such as AutoCAD Lite should be able to accomplish the basic .DXF preparation.

I have seldom received a .DXF file which contains exactly what I need and nothing more. Instead the file is flooded with
layers that has no meaning for the layout engineer. The content of unused layers should be deleted and the layers
should be purged before an import is attempted.

If you have no access to a .DXF editor, then cross your fingers and hope that the layers in the .DXF are prepared.
Layer 0 (zero) is always present. Other layers can have arbitrary names and these will appear in the import menu.

As the import procedure is initiated, you will be given options how to map the layers present in the .DXF.

If the layers are clearly named, just map them to the layers present in the Allegro editor. If you find layers
that you may want to keep, map them to a Drwaing_detail or something similar. Texts can also be mapped
to documentation layer, as these texts may not appear correctly in silkscreen etc. Slots or cutouts can be
mapped to the BOARD_OUTLINE but remember not to map drill holes or slots in pads. They need to be defined
in the drill and route file. One solution is to locate all mechanical drill holes, add them in the schematic to a
layout symbol (footprint), connect the hole to GND (if it has to be tied to a net) and then do a forward
annotation. Then place the holes right where the holes appear in the documentation layer in the .BRD-file
(assuming that you just imported a .DXF-file into it).

You should select "Incremental" import, as otherwise Allegro layer structure will be overwritten.

And remember: The unit of measure in the .DXF must be the same as in the .BRD-file.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top