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

[agaribay]

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

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[pfariello]

Interesting question. I have been struggling with company drawing standards which are requiring all parts to be "fully" dimensioned on the print. I personally feel this is impractical if not impossible for many injection molded or die cast parts that have any type of free form surfacing.

I would be interested if anyone works under the premise of a "fully" dimensioned print and if it is acceptable to reference the database to confirm or measure feature size.



ALL NOMINAL PART GEOMETRY IS DEFINED BY THE PRO/ENGINEER DATABASE. ALL
FEATURES NOT DIMENSIONED SHALL BE REFERENCED FROM THE PRO/ENGINEER DATABASE.
ALL POINTS IN THE DATABASE MUST BE HELD TO THE LINEAR TOLERANCE SHOWN IN THE
TOLERANCE TABLE ON THIS DOCUMENT.

Regards,
Patrick Fariello
CommScope
1300 E. Lookout Dr. Suite 150
Richardson, TX 75082

[JoseResendis]

Hi Patrick,

Similar to your note below, the notes on our "Limited Dimension Drawings"
reference an internal tolerance spec doc in addition to the note that
points to the cad file.

Best Regards,

Jose M. Resendis
Mechanical & Optical Engineering Center (MOEC)
Raytheon - Space & Airborne Systems (SAS)
972-344-2555 office
972-979-5525 cell

"Great execution requires discipline"

[ptc-141274]

This is what we use for what we call “virtual drawings”. We will generally dimension holes for hardware, and anything we consider critical / want inspected.

~Doug



&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&

3. TOLERANCE ON ALL UNDIMENSIONED FEATURES
SHALL BE: Profile Symbol | .010 | A | B | C |

3.1 TOLERANCE OF ALL DIMENSIONED
FEATURES SHALL DEFAULT TO TOLERANCE
BLOCK UNLESS OTHERWISE SPECIFIED.
3.2 DEFINITION OF ALL UNDIMENSIONED
FEATURES SHALL BE PER ELECTRONIC
DATA FILE: md_xxx-yyyyyy-zzzz_-.
THE 10 CHARACTERS FOLLOWING "md_" REPRESENT
THE PART NO., THE NEXT 5 CHARACTERS
REPRESENT THE CONFIGURATION, AND THE LAST
CHARACTER (OR LAST 2 CHARACTERS) REPRESENTS
THE REVISION OF THE DATA FILE AND DRAWING.
3.3 DIMENSIONED FEATURES TAKE PRECEDENCE
OVER THE ELECTRONIC DATA FILE.
3.4 THE REVISION OF THE DRAWING AND
THE ELECTRONIC DATA FILE SHALL BE
THE SAME.

&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&&

[jflores-3]

We do pretty much the same, only dimension interfaces and design requirement critical features as well as when required add a dimension here and there to statistically monitor the process. Our model note is kind of simple:

ASSOCIATED ELECTRONIC DATA SET &model_name WITH SAME REVISION
AS THE DRAWING FORMS A PART OF THIS DOCUMENT IN THE EVENT OF A
CONFLICT, THE ELECTRONIC DATA SET SHALL TAKE PRECEDENCE.


Thank you, Jim Flores
Mechanical Designer / CAD administrator
Sustaining Engrg, Philips Healthcare, PCCI
Hospital Respiratory Care
2271 Cosmos Court
Carlsbad, CA. 92011
-<">mailto:->

[pfariello]

A few more questions,

On either the "Limited Dimension Drawing" or the "virtual drawing", how are these drawings used? Is it acceptable to release for production?

If there was a discrepancy on a delivered piece part where the feature was not explicitly dimensioned on the print, is it acceptable to use the database as the reference to show the discrepancy?


Thanks,
Patrick Fariello

-<blocked::<a style="COLOR:" blue;=" text-decoration:=" underline&quot;=" target="_BLANK" href="mailto:-">">mailto:->

[JoseResendis]

Since the drawing states that dimensions not shown on the print are derived
from the cad data file, You then
use the cad file to settle any discrepancies. As for whether its
acceptable for production would depend on
your supplier's capabilities. The majority of shops are using the cad data
for producing parts these days
even if they take a translated version of your native cad file and generate
an in house drawing for their needs, they
are still using your model.



Best Regards,

Jose M. Resendis
Mechanical & Optical Engineering Center (MOEC)
Raytheon - Space & Airborne Systems (SAS)
972-344-2555 office
972-979-5525 cell

"Great execution requires discipline"

[DamianCastillo]

This is a very interesting topic.

In some cases our drawings are the only documentation we can send to production and in other cases we can send the model and the parts are made by CNC. When you are dealing with complex geometry, it is difficult to fully dimension the drawings which poses a problem in some cases.

If the drawing is approved and has a signature, how do you determine if all dimensions were looked at when the decision was made? If the drawing does not contain all the dimensions to define the product, how do you insure the model was analysed during the approval process?

Some have suggested using GD&T which has a Surface call out that will let you point to a complex surface and state that surface must be within a particular tolerance range of that shape to be acceptable. Now the question is, how do you measure it and how do you document it was done correctly when approving the drawings?

This is a challenge for us as well and we are trying to find the most realistic approach that defines the product without having to create many cross sections to define complex geometry areas.

We don't officially use the 3D Drawing standard and do not annotate our 3D models but this seems to also be an option. The problem we have is that in some instances we can only provide a 2D Drawing for production and not a 3D model.

I would love to get some feedback and ideas from others about this.

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

[Brndn_4]

I'm not really savvy with inspection, but can't you inspect the physical part with CMM and directly compare it to a model? We use FARO tools here depending upon need. I don't know the details, but it seems to suffice for complicated profiles that would otherwise require point sets and sections with tolerancing. I think some of our vendors do it as well since they use neutral files for machining.

In Reply to Damian Castillo:

This is a very interesting topic.

In some cases our drawings are the only documentation we can send to production and in other cases we can send the model and the parts are made by CNC. When you are dealing with complex geometry, it is difficult to fully dimension the drawings which poses a problem in some cases.

If the drawing is approved and has a signature, how do you determine if all dimensions were looked at when the decision was made? If the drawing does not contain all the dimensions to define the product, how do you insure the model was analysed during the approval process?

Some have suggested using GD&T which has a Surface call out that will let you point to a complex surface and state that surface must be within a particular tolerance range of that shape to be acceptable. Now the question is, how do you measure it and how do you document it was done correctly when approving the drawings?

This is a challenge for us as well and we are trying to find the most realistic approach that defines the product without having to create many cross sections to define complex geometry areas.

We don't officially use the 3D Drawing standard and do not annotate our 3D models but this seems to also be an option. The problem we have is that in some instances we can only provide a 2D Drawing for production and not a 3D model.

I would love to get some feedback and ideas from others about this.

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

[DarrinHiebert]

I haven't been following this topic faithfully, but today for some reason,
it caught my eye, maybe because I'm too busy learning WindChill. 😉



We do something very similar to what the other posters have said, we have
a note that says something like this:



ALL FEATURES NOT SPECIFICALLY REFERENCED OR DETAILED ARE CONTROLLED BY CAD
GEOMETRY.



I don't know that this really "does" anything for us, but it definitely
makes us feel good!



To Damian's question, however. One way that we "control" this is with
CMM. It's not really control per se, but it is a way for us to verify
that the shape is what we want. With that being said, we have features or
areas on parts that we cannot accurately measure with our CMM vs. the
model. Fortunately, for us, those unmeasurable areas are not critical to
fit, form or function, so we don't measure them.



With all of that being said, we always dimension those areas that ARE
criticial for form, fit, function, or location, and sometimes, those are
NOT easy to detail on prints.

[mlocascio]

I am not sure about the origin of this stream either, but I will put in my
plug for using the model the way that Pro/E intended the model to be used. I
just came from an environment where it seemed like models were only good for
one thing - adding dimensions. I am a strong advocate for making the model
reflect what is desired for manufacturing. When done right this means that
any change that I want done in a model can be done in the drawing and visa
versa. The only time that we as Pro/E users should add dimensions is when
there is no other way to describe the geometry in question.



It's kind of a simple principle, my fellow Pro/E users, we are using Pro/E,
not AutoCAD. If you want to produce AutoCAD quality drawings there are much
cheaper ways to do that. Use Pro/E as it was intended to be used. It makes
it easier for those who have to work with your stuff later.



Michael P. Locascio

[DamianCastillo]

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"

[mlocascio]

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.

[DamianCastillo]

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"

[MikeFoster]

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.

[pfariello]

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

[pfariello]

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

----------

[MikeFoster]

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