Skip to main content
A
agaribay1-Visitor
1-Visitor
January 24, 2013
Question

“…dimensions not shown on drawing are controlled by 3D CAD File…”

  • January 24, 2013
  • 17 replies
  • 25901 views
Hey guys,

What is a standard drawing note you would use for complex models that require the 3D Model to complete the drawing?


Something like:

“…dimensions not shown on drawing are controlled by 3D CAD File…”

Thanks.

-Art

.

.

.

.

This message (including any attachments) contains

confidential and/or proprietary information intended

only for the addressee. Any unauthorized disclosure,

copying, distribution or reliance on the contents of this

information is strictly prohibited and may constitute a violation

of law. If you are not the intended recipient, please notify the

sender immediately by responding to this e-mail, and delete the

message from your system. If you have any questions about this

e-mail please notify the sender immediately.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

17 replies

Show previous replies
D
DamianCastillo1-Visitor
1-Visitor
January 25, 2013

Very good points and I forgot to mention that we have a 3D Laser Scanner that we use to verify First Article Samples.


We approve a sample after comparing the 3D Scan model to the CAD model and we have a report generated with Geomagic Qualify that we can refer to in the future as needed.


My biggest concern is the note or dimension on the drawing that gives you some sort of standard to go by when you can't send a 3D Model to production and they must rely only on the 2D Drawing.


We can verify after the fact if the part passes but during production, it's difficult for the 2D Drawing to convey the complex geometry using dimensions.


If they are not able to use the 3D model to CNC the part or in our case the molds, what could we provide them on the 2D Drawing to clearly define the complex geometry they are trying to create?



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

M
mlocascio1-Visitor
1-Visitor
January 25, 2013
I would think that if you have a good CAD model that would be what guides
the produced piece. The drawing that you use to accompany will have
inspection dimensions or critical dimensions that have been discussed with
the vendor or manufacturer.


D
DamianCastillo1-Visitor
1-Visitor
January 25, 2013

Michael,


We outsource products all over the world. In some cases you can't provide a model and only a 2D Drawing. This is where the challenge is.


We have a good process for sending 3D models to manufacture a product and although it's usually the normal process, it's not always an option.


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

M
MikeFoster10-Marble
10-Marble
January 25, 2013

All,

We’ve been creating what we call partially defined drawings for a few years now. Below is our definition and rationale.

Mike Foster
ATK


A Partially Defined Drawing (PDD) is a drawing that has been simplified in that it does not contain a complete set of dimensions and views. For complete product definition the dimensional information is queried from the model geometry contained in the CAD digital data file.

A PDD is identical to a fully defined drawing with the exception of the following:

1. Basic dimensions are not shown on a PDD and are to be queried from the Design Model (CAD digital data file).
2. Drawing views are not necessarily present to show all surfaces in their true shape.
3. A note and stamp define the drawing to be a PDD.

All other dimensions, tolerances, notes, etc… are shown as on a fully defined drawing.

A key element of a PDD is the "Default Profile" – a relatively loose, unless-otherwise-specified, GD&T profile tolerance that applies to all features that do not have their tolerance explicitly defined. The Default Profile appears on the face of the drawing in one of the drawing views and is designated by use of the annotation "ALL OVER UNLESS OTHERWISE SPECIFIED"

The following note is placed on all PDD drawings. It specifies the data file name and that the geometry represents the nominal size (perfect form).

DESIGN MODEL IS REPRESENTED IN REVISION-CONTROLLED CAD DIGITAL DATA FILE WITH NAME FORMAT: PART NO_REVISION_3D.STP. DESIGN MODEL REPRESENTS PART AT NOMINAL SIZE BEFORE FINISH. VALUES QUERIED FROM THE MODEL ARE BASIC UNLESS OTHERWISE SPECIFIED. INTERPRET PER ASME Y14.41-2003.

PARTIALLY DEFINED DRAWING. THIS DRAWING SHALL BE USED WITH THE DESIGN MODEL FOR COMPLETE PRODUCT DEFINITION. QUERY OF THE MODEL IS REQUIRED FOR UNDIMENSIONED FEATURES.


Rationale for definition of a PDD:

A piece part defined by a PDD must have a defined, unambiguous tolerance for every single feature or surface on the part just as a part with a fully dimensioned drawing does – This is a fundamental requirement of ASME Y14.5 Dimensioning and Tolerancing. A PDD must fully comply with the requirements of ASME Y14.5-2009 and ASME Y14.41-2003.

Traditional or X-Y type dimensions cannot be left off a drawing because there are multitudes of ways in which a given feature can be defined by an X-Y dimension. For example; features can be dimensioned either from one end of the part or the other; successive features can be dimensioned either as coordinate dimensions or serially from one to the next; etc… A PDD with X-Y dimensions left off therefore fails the requirement that every feature have a single unambiguous tolerance.

Basic dimensions on the other hand do not define tolerances. Basic dimensions by definition describe the theoretically exact size, profile, orientation, or location of a feature whose tolerance is defined by GD&T feature control frames. As such, a basic dimension can be queried from a Design Model (CAD digital file) which is a theoretically exact geometric representation of a part.

A PDD piece part's tolerances, by design, are predominantly defined by GD&T. This enables the majority of its dimensions, were they present, to be basic.

PC-DMIS is an example of automated digital inspection software that can deal with PDD's.



P
pfariello1-Visitor
1-Visitor
January 25, 2013
I somewhat hijacked this thread when the question was asked about a standard print note to reference the CAD model. My reply of which many of you shared a similar method was a call out to the model and a reference to a tolerance range for the features. Some said the model superseded, while some said the print superseded.

I was hoping to expand this to understand what other companies did/ allowed in regards to referencing the CAD database for features that are not explicitly dimensioned on the print.

In my previous life, the philosophy was that the CAD model was gospel. This is where the design was constructed, it contain the design intent. The print was a vehicle to detailed inspection points and other relevant information.

I work with many part/ process types, injection molding, die casting, PCBs, die cut, sheet metal form and precision metal stampings, machining. Across all these areas, some suppliers have to work from the database, while others do not have CAD and will work from the print. It would be comical to think the injection mold tool builder would build off of the print, but for the vendor making "L" brackets this might be ok.


The original question,
"What is a standard drawing note you would use for complex models that require the 3D Model to complete the drawing"


Damian alludes to some of the same issues that I am experiencing in my new life.

If the vendor does NOT use CAD, can you still hold the vendor to the CAD model if the feature is not defined on the print?
If the vendor DOES use CAD, can you still hold the vendor to the CAD model if the feature is not defined on the print?



Thanks for everyone's inputs.
Patrick Fariello
P
pfariello1-Visitor
1-Visitor
January 25, 2013
Hi Mike,

Is the PDD acceptable to release for production?

Is the PDD stand alone, or is there an additional drawing for the part?  You state "All other dimensions, tolerances, notes, etc... are shown as on a fully defined drawing." , so  I was not clear on your full use of the PDD.

Thanks,

Patrick Fariello

----------
M
MikeFoster10-Marble
10-Marble
January 25, 2013
Hi Patrick,

According to ASME Y14.41-2012 there are two items that make up the complete product definition:


1. Model - This is the 3D CAD digital data file - (It is either Pro/E or STEP format).

2. Drawing Graphic Sheet - We call this item the PDD - (It is either a Pro/E drawing file or a PDF).

Both of these items are required to release for production.

If you took a traditional fully dimensioned 2D drawing and erased all the basic dimensions and unnecessary drawing views you would be left with a PDD. Therefor the PDD cannot stand alone because it is missing information that is now provided in the Model (3D CAD digital data file).

Thanks,

Mike

Terms & ConditionsCookie settingsAccessibility statement