Pro/ENGINEER Support

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In this age of increasing competition, cost and time to market are two very critical factors that all OEM's must seriously address. PTC's suite of products allows an efficient flow of digital data between a company and it's vendors. Fully implemented, this is a powerful product development system for taking products from concept to the factory floor.

One step where this system is often broken is in communicating manufacturing information to a machining vendor. It is common to create translated versions of a model (i.e. - IGES, STEP, DXF) and to create fully dimensioned drawings for the sake of a vendor that is not Pro/ENGINEER capable. These practices introduce both unnecessary cost and time. While making 2D drawings is sometimes a necessary step in the process, it is tedious, usually non-value added, and lengthens the cycle. Once a drawing is put on paper or a translated version of the model is made, the intelligence and associativity of the model is lost and the power of Pro/ENGINEER is diminished.

Pro CNC has developed a system with which customers can eliminate the need to create 2D drawings, and rather embed this information into the native Pro/E model. Below, we discuss some basic techniques that can be used to reduce or eliminate the need for creating 2D drawings when transferring product data to Pro CNC. We then can open your Pro/E part model in Pro/MANUFACTURING (Pro/NC) and extract the relevant manufacturing data.

Transferring files by email or FTP site

The method of transferring files can either lead to a lot of confusion or it can be really smooth. By using a zipping utility and the naming convention of XXXXX_rev-$.zip (where XXXXX is the part number and $ is the current Rev of the part inside.) it is plainly clear what part number and rev. is being sent. All subsequent zip files with a new rev part should have the rev incremented appropriately.

Config.pro Options

The config.pro file must be set up with the correct options to be able to communicate well without a print. Below are some options that we recommend:

Tol_mode - Nominal
Linear_tol_0.xxxx - make applicable
Angular_tol_0.xxxx - make applicable
Tol_display - yes
Pro_unit_sys - if metric, make custom – mm, grams, sec.
Template_solidpart - browse to pick model
Model_tree_start - yes
Start_model_dir - browse to “templates” dir. or correct dir.
Accuracy_lower_bound - .0002
Default_dec_places - use most common ie 3
Sketcher_dec_places - use same as default_dec_places

Embedding information into your Pro/E model
There are several places where part information can be embedded into the model:

Parameters are a great place to include information such as:
- Part Number
- Description
- Rev
- Material
- Engineering Contact

Notes can be used to communicate items such as:
- General Company and or Workmanship Notes
- Proprietary Notice
- Finishing Specs (such as anodizing, chem film, etc.)
- Rev History

There are several very important modeling and part setup considerations:

Tolerances:
-Always model to the nominal dimension, and if at all possible use symetrical bilateral tolerances. Do not put unilateral tolerances on a part. i.e. - If you want a bore to be 0.500" +.004, -.000 then model and tolerance it 0.502" +-.002. If you use unilateral tolerances then programming from the solid model and holding tolerances becomes much more difficult.
- Use correct linear tolerances from config.pro
- Use correct # of significant digits
- Modify dimensions that need a non-standard tolerance and apply the correct tolerance. You can then show which features have a non-standard tolerance placing an X next to the feature in the model tree. (see below)

Gtols:
- Specify Datums
- Apply Gtols to appropriate dimensions

Other ways to communicate information:
- Apply surface finish requirements to individual surfaces (i.e. - 32 microinches)
- Specify threaded holes by using a hole feature and selecting the correct threads or by using cosmetic thread features and make sure to fill out all appropriate attributes.
- Specify inspection dimensions by placing an X next to the feature in the model tree.
- Part Marking can be specified with a Datum Curve box to show location and size.
- Read Only - Pick the last feature on the model to make all features uneditable. (good practice to make sure features aren't accidentally changed)
- Suppressed Features - Try not to have any if possible. They are just sources of potential error.
- External References - Freeze them so that the dependent does not need external refs.
- Model Tree - Add new columns to the model tree called sp_tol and inspect. Columns can be added by the following menu options on the model tree. Tree; Column Display; under the type drop box pick Feat Params; type in sp_tol in the name box and click the arrow to add it to the displayed list. Repeat for inspect. Format the columns to be 3 characters wide each. You can save the tree file (tree.cfg) in your Pro/E loadpoint so you don't have to do this again. Then you can place X's next to any feature you want to be inspected or that has a non-standard tolerance that isn't covered by the tolerance block.

Please feel free to call us if you have any questions at all about this information. We will be happy to go over any specifics that may or may not apply to your situation. Our phone number is 866-4PRO CNC (477-6262). Or drop us a note at: .(JavaScript must be enabled to view this email address).