Gerber files

You are right creating the .art files for Gerber.

For soldermask you need to set the classes and subclasses in the color and visibility window. Switch ON the subclasses that you need under each class.

Add new film in the Artwork for Soldermask Top say Mask_Top. Right Click on the Mask_Top and say match display. What ever you set on the color and visibility is now a part of this artwork. You can now save this (.art) file.

Similar is the case with Soldermask Bottom.

Hope this helps you.

You are right creating the .art files for Gerber.

For soldermask you need to set the classes and subclasses in the color and visibility window. Switch ON the subclasses that you need under each class.

Add new film in the Artwork for Soldermask Top say Mask_Top. Right Click on the Mask_Top and say match display. What ever you set on the color and visibility is now a part of this artwork. You can now save this (.art) file.

Similar is the case with Soldermask Bottom.

Hope this helps you.

Regards,
Kishore

I highly reccomend you review the Online documentation, Allegro PCB Editor User Guide: Preparing Manufacturing Data, Product Version 15.7

It details all the steps for creating artwork etc...

Shown below are the detailed steps from CDSDDoc for creating film records

Creating Film Records for a Gerber Data File
To produce artwork data files, the editor reads the film control records that you create in a layout. It reads these records to determine the following:

The number of artwork files to produce
The names it assigns to the artwork data files
The classes and subclasses to include in each artwork data file


Run the color command or Display - Color/Visibility to display the Color and Visibility dialog box.

In each group (Geometry, Manufacturing, Stack-Up, Components, and Areas), turn off all the classes and subclasses and then choose the classes and subclasses that you want included in the Gerber data.

Run the film param command or Manufacture - Artwork.

When the Artwork Control dialog box initially opens, it reads the cross-section and auto-generates one film record for each etch subclass. The record consists of etch, pins, and vias. Once you click OK in this dialog box, the editor does not automatically update the list again.

To add a new record, right-click one of the film records listed in the Available Films list.

Choose Add from the pop-up menu.

In the New Film field of the dialog box that appears, enter a new film name for the Gerber data file and then click OK.

Repeat steps 4 to 6 for any other film records that you want to create.

You can manipulate the film records and layers by right-clicking the record or layer and choosing options from the pop-up box.

Complete the Film Control tab of the Artwork Control Form dialog box.

Choose the General Parameters tab and set the photoplotter model type and associated parameters.

When you have completed setting all the parameters in both the Film Options tab and the General Parameters tab of the Artwork Control dialog box, do one of the following:

Click Load to add a previously created film record text file.

Click Create Artwork to generate artwork for the films you have selected.

Click OK to close the form.

[b] [/b]

 Just wondering, are .art formats the same as .gbr ? Which means if i give the PCB house (they accept Gerber, Gerber 274X and ODB++)  .art (Top.art and Bottom.art) and .drl files, can they do the fabrication? Or is there a software that converts .art to .gbr?

 I am new to PCB design so i am not familiar with the different formats.Thanks.