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commandments of pro/e

23-Emerald II

commandments of pro/e

My friday topic is a request. Years ago, someone sent out or I came across a "ten commandments" of pro/e. Things you shouldn't or should do.

Stuff like "thou shall not sketch all features in one sketch" and "thou shall only use shown dimensions" (no, please, no, don't send any emails on created vs. shown dims)

I think it would be good to share it with my co-workers here.



"Thou shall not use cosmetic sketches"

They bleed through everything, can someone please give me a use for

Feel free to contact me with any questions

Bill Samuels

"Thou shalt not use family tables for anything accept a true family,
such as fasteners."

Any other usage, and the lord thy PDM administrator shall cast a curse
of "legacy drawing conversion" upon you and 3 generations of your


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They do have 2 advantages I can think of....

1. They do not have to be constrained at all (you can exit the sketch
without a dimension). The value? Maybe none?

2;. You can erase it from any view. I like this better than dealing with

One negative .... you can't dimension (piggy-back) off of them.

I have not used the feature in a things may have changed.

The bleed factor does make me lean more towards NOT using them. This feature
looks like it would be phased out eventually in the software.

Back in the day... (version 15) when I learned Pro/E, I was told the following:
1. Try and keep your sketches to no more than about 8-10 dimensions.
2. Try to keep all the small rounds towards the end of the model.
3. When re-defining features with drafts and rounds and you remove a reference to cause a warning of a child feature - fix the missing references right away to avoid issues down stream.
4. When modeling features, always "try" to reference MAJOR datum planes (i.e. FRONT, SIDE etc...) instead of other features.
5. When creating parametric parent/child components in an assembly, ALWAYS use surfaces and NEVER the edges of the parent part.

I'm sure there are more, but these come to mind right away.


One of my biggies:

Thou shall never reference a model edge if there is a suitable surface

Doug Schaefer
Doug Schaefer | Experienced Mechanical Design Engineer

I got this off the exploder a long while ago... don't know from who...
but FWIW...

Commandments of Pro/E

(These are good generalized rules downloaded from a Pro/E user group
email. Note: As in life there is no one way to do something and there
is no one rule to explain everything)

Part Mode

* Thy Holes and cuts shall not be filled.

* Thy Features shall not be covered completely by other features

* Thou shall add chamfers, drafts, and rounds at the end of the model
and not create children of chamfers, drafts, and rounds

* Thou shall avoid creating rounds and chamfers in sketcher, as they
should be added as separate features, when possible.

* Patterns shall be used in preference to copy

* Thou shall keep sketches simple and not create complex features with a
single sketch

* Thou shall name thy features to ease future redefinition

* Incomplete features shall be removed or completed

* Thou use thin sections when applicable

* Thou shall always keep the same parent surface for thy merges.

* Thou shall use datums to define depth of feature when feature depth is
likely to change, and feature will have plenty of children

* Thou will have problems with drafts and rounds

* Thou shall reference datum features in sketches wherever possible

Drawing Mode

* Thou shall not use Snapshot, unless required in dire need

* Thou shall use shown dimensions as much as possible

* Only Company standard formats shall be used on drawings

* Thy drawings shall not contain overwritten dimensions (@o)

* Models attached to Thy drawings, but not showing in any views, shall
be removed

* Thou shall Orient views using default datums or view names, not thy
model geometry

* Thou shall make the drawing independent of local environment settings

Assembly Mode

* Thy alternative components shall not be left assembled on top of each

* Thy Assembly features, such as cuts, shall be avoided

* Thou shall use constraints that reflect real-life assembly or
manufacturing situations

* Thou shall follow the rule that assembly datums make the best parents

* Thou shall not select constraints simply based on ease of selection of

* Thy Frozen components shall be resolved


* Thou shall not submit parts and assemblies to IntraLINK with
suppressed feature and components

* Thou shall not submit parts and assemblies to IntraLINK in insert mode

* Thou shall verify all instances before Check-In


* All thy applicable parameters shall have a value assigned

* Thou shall orient sketches the same way within a model e.g. always set
HOR or VER as "TOP".

* Thou shall use start parts & Assemblies for all new models

* Thou shall clearly comment all relations

* Thou shall learn to love Layers and his more advanced brethren,
Simplified Rep's

* Thou shall not make any unintended parent-child relationships or you
will suffer the wrath at the hands of redefine, reroute, and reorder.
The use "query select" or "select by menu" shall be used if there is any
doubt as to which entity you are selecting, to ensure correct
parent/child relationship

* Thou shall use the erase option to clear objects from memory and shall
not be confused with the delete option.

* Thou shall save early and often

* Thy Circular References shall be resolved

* Thou shall learn to create multiple datums-on-the-fly

* Thou shall limit points on splines.

* Thou shall save parts with axes, points, surfaces, planes, geo tol,
coords, blanked.

* Thou shall consider too many datum features (planes, curves, points)
as never enough and unused datums shall be deleted

Paul Korenkiewicz
FEV , Inc.
4554 Glenmeade
Auburn Hills, MI, 48326-1766

I was thinking of getting these framed up in one of those
"inspirational" posters you see in the lunchroom... Then I could sell
them for $100 each and retire! ... Oh, btw, included with each poster
is a cattle prod for those that need some gentle persuasion...

yes, it's Friday... and I need my turkey ruben!!! 😉

Paul Korenkiewicz
FEV , Inc.
4554 Glenmeade
Auburn Hills, MI, 48326-1766

The attached .doc are what had been sent earlier consolidated with a couple more added. I then formatted it to print nicely on 11x17 paper.


--- On Fri, 2/27/09, Korenkiewicz, Paul <-> wrote:

We create cosmetic sketches to indicate areas that need to be masked before coatings get applied. Then blank them on the parts and show them in the appropriate views on the drawing.

23-Emerald II

Thanks to all who responded. Carrie was nice enought to do most of the summary and actually make it look nice. I would have been too lazy to actually do any formatting (thou shall not be lazy in thy modeling!!).

Tom submitted his top 11 list. He also included explanations, which for new users is especially helpful since some of the terminology changes over the years. I like the reference to "part mode", "assembly mode", drawing mode"...a reference to theDBMS menu would have been the bomb.

Don't create buried features was a common response. And Gerry placed a curse on all who used family tables to create objects that weren't true families.

It's always a good idea to remind your users, new and OLD, about good modeling practices.

Thanks to all who responded,


Now with Wildfire 5.0 allowing you to skip Resolve mode. We need to add one.

Thou, shall not leave unresolved features in the Model Tree. (Red Text Features)

Just looking ahead.

"Too many people walk around like Clark Kent, because they don't realize they can Fly like Superman"

WF5 allows unresolved regeneration errors?
How is this possible?

Will it be possible to check them in into Windchill? With unresolved

If something has to change regarding Resolve Mode, then it the
Pre-Wildfire functionality. Only Quick Fix is used, since Fix Model
only allows to access features in ancient pre-Wildfire menu's.

Regards, Hugo.
Business Continuity with Creo: Learn more about it here.

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