Good modeling practice.

[jabbadeus]

rcamp's right, I meant to say that DRAWINGS should have >95% of the dimensions as SHOWN dimensions.



Here's why this is recommended as a good modeling practice:



1. Showing dimensions is a heck of a lot faster than inserting dimensions when creating a drawing.



2. If the part ever changes, then the shown dimensions will update appropriately. If one has mostly inserted/created dimensions, then you might see the drawing blow up (dimensions turn purple because references disappear, etc.). Shown dimensions should reduce the amount of work you have to do to the drawing when the part changes.



Note that one should NOT go back into a part and redefine features in order to be able to show those dimensions on the drawing.



Like kvision said in his first point, think first, then model. Hopefully designers are choosing a dimensioning scheme that relates to how they want to control their model; hopefully these dimensions also relate to manufacturing and inspection. (rcamp, it sounds like due to the nature of your design procedures, your designers don't have the time or opportunity to practice this.)



And I also hope that production drawings go away in favor of managing through models. (A 2-D production drawing always seems to me like a step backwards once you have a good 3-D model. Whenever I say that though, I tend to get a lot of people arguing with me.)

 

[airion]

If you specify any holes in your design, create them as

hole features and not cuts. One exception are

compound holes - these can only still be created as

revolved cuts (misfire may be different, anyone

know ??) dougr



I saw this mentioned a couple times, but I don't see a reason for it. What is wrong with using a cut feature to make a hole?



I can see where the opposite is bad, i.e. trying to redefine a hole into a non-circular shape only to find out it is a hole feature and not a cut.



Al

 

[kvision]

If you are a small company and few people will see or use your drawings then shortcuts like not using shown dimension may be appropriate especially for molds and castings which often need multiple steps shown.

HOWEVER in a concurrent engineering environment where drawings are OFTEN passed from designer to designer SHOWN dimensions prevent errors. HOW? A created dimension can be overwritten with @O. This usually shows it's ugly head when a second or third hand user decides to change the dimension on the drawing instead of fixing the model. The drawing APPEARS correct but in fact the model isn't correct. This can lead to manufacturing problems and INCORRECT parts being delivered. There will always be reasons to skirt the good/best practices and MONEY is almost always the number one culprit. Number 2 is usually because you are doing a 1 of part and don't expect to ever reuse the model. Then of course years later you need to and then you must completely rebuild the model because the lack of capturing the original design intent has led to insurmouontable complexities in the model/drawing.

SHOWN dimensions are ALWAYS the best idea IF you can get them. You can check each drawing/model as it is submitted by running modelcheck on it and checking for created dimensions and then deciding if they are necessary or not. I have seen extremely expensive mold/cast/machined parts get scrapped because someone used @O to fake something and it never got caught. It happens.

Ever had to do a 500K qual test on part and then find out the part was wrong and must be re-qualed because dimensions were faked on the drawing but the solid model was used for down stream manufacturing?

A good rule of thumb about doing something is this. Ask yourself, Would it be ok if I did everything this way?

ie. Should I fake/create all the dimensions? Should I overwrite all dimensions without updating the model?

Should I NOT be concerned with constrining any my sketches correctly? BTW- If you don't care how the sketches are constrained or dimensioned, how can you be sure that it will update or move correctly when you change a dimension?

As for going back to redefine sketches to get shown dimensions. the answer, IMHO, YES, if the model will be reused over and over in the future. NO, if it's a 1 or 2 of part.

 

[dougr]

btw have any of you ever thought about what would happen if drawings were eliminated and we therefore couldn't rely on driven dimensions to convey design intent ???

 

[kvision]

I saw this mentioned a couple times, but I don't see a reason for it. What is wrong with using a cut feature to make a hole?





Nothing is WRONG about it but a hole is a pick and place feature and no sketching is required. This makes it faster to make a hole rather than a sketch. Holes regen faster as well.

 

[kvision]

btw have any of you ever thought about what would happen if drawings were eliminated and we therefore couldn't rely on driven dimensions to convey design intent ???



Yes. Model release is the future of manufacturing and is a perfect example of why the model should be thought out, correctly dimensioned and constrained in every sketch and all manufacturing data such as GTOLs, tolerances, finishes, etc should be included in the part model. Also if you want to use automation/program/toolkit in part/drawing creation then SHOWN dimensions are perfectly suited to this as are predefined views, etc.

 

[dougr]

kvision,



Thank you for restoring my sanity...



What is wrong with using a cut feature to make a hole?



Don't hole features contain additional information for pro man also ??

 

[dr_gallup]

I very much disagree with rcamp about certain statements:



Assuming he means your DRAWING should have > 95% of the dimensions as SHOWN dimensions, I would say this statement is restrictively dogmatic. Shown dimensioning is a nifty idea that has very little practical use, IMHO.



I ALWAYS try to use shown dimensions and try to dimension my sketches with the drawing in mind. I DO go back and redefine sketches if needed to get the correct dimensions to show in the drawing. The reason is drawing modifications are so much easier next year or next DECADE. Yes we have ProE models more than 10 years old. It is so much easier to modify something if I can just change the drawing dimension and the part regens as I expect.



Another problem with using shown dimensions is that assembly feature dimensions can not be shown in a view of a part model. Only part feature dimension can be shown in a part model drawing. Should I give up the power of assembly features so that I can use shown dimensions? Why would I give up such a productive capability for something that doesn't even save time?



Assembly features should only show up at the assembly level where you can show these dimensions.



We are a manufacturer of plastic injection molds. We build from 3D data (ProE models about half of the time). We don't see our customers prints until we are through building their parts! Therefore, any effort to reflect anything other than inspectional requirements is an absolute waste of time (and obviously we don't need them to build the tooling).



This is total BS unless you are building tooling for parts that have no critical tolerances. We never release a part for tooling without fully detailed drawings because we have very high requirements. If you build a tool for us without taking the tolerances into account you will be eating that tool!



I agree that asymmetric tolerances are a bad idea for most parts, molded or not.



Except for the simplest assemblies or parts that are not used in assemblies, it is illogical to drive models from drawings. What is the purpose? The only purpose I see is to enable someone unfamiliar with the model to be able to make changes to it from the drawing, but that person probably shouldn't be changing the model anyway, since they wouldn't know what affect it might have on other features.



I find it helps me a great deal when I have to revisit a model after a few years.



Does any one else find using shown dimensions a useless concept? Does anyone else see drawings/prints approaching obsolescence in the reality of the manufacturing world?



The reality of the manufacturing world is that drawings will be with us for years to come. We need drawings to RFQ vendors, we need drawings for incoming inspection, we need in-process drawings and we need drawings for our customers. Other than mold makers I have yet to find a supplier that could use a 3D model. And I don't trust the mold makers that think they only need a 3D model.



The only real output of an engineering department are the drawings and specifications that define a product. It doesn't matter if you produce them with Pro/E or stone tablets and a chisel. The stone tablets might be more durable in the long run.

 

[rcamp]

I think a clarification and distinction needs to be made, if I understand the comments made so far.



Manually altering a dimension by using @0 and manually creating a dimension a two VERY different things. It appears to me that several people are speaking of them as the same thing. I was not. Manually altering a dimension by using @0 is the same as lying or cheating and someone should be terminated for doing, this should absolutely not be tolerated as an acceptable practice. Configs might could be used to absolutley prevent this, but basically, its sabotage, you CAN'T prevent, you just have to trust the people you work with.



The amount of time it takes to manually create a dimension is not significantly differently than the time it takes to show a dimension. The bigger issue, again, is Only part feature dimension can be shown in a part model drawing, no one seems to recognize the power of assembly level modeling!

 

[rcamp]

dr_gallup said:





This is total BS unless you are building tooling for parts that have no critical tolerances. We never release a part for tooling without fully detailed drawings because we have very high requirements. If you build a tool for us without taking the tolerances into account you will be eating that tool!





We don't have a problem building molds for customers like you. We build the way our customers want. If you have the luxury in your industry that you can wait to release tooling until you have finalized prints, that is wonderful. That is what we prefer. I am just telling you what most of customers do. They say we have to have parts in 5 weeks knowing that they are not going to have prints done. They want us to start anyway usually because they don't have the luxury of time, it is a VERY competetive marketplace, and often the first one to market is the successful one. We help them accomplish their goals by having the ability to build accurate tools without prints. I there is something that require more than can be met by typical industry standards and practices, it is their responisibilty to communicate that to us, by whatever means.

 

[jabbadeus]

>> The amount of time it takes to manually create a dimension is not significantly differently than the time it takes to show a dimension. <<



For a single or handful of dimensions, this is true. But for a part with more than a couple dozen dimensions, a person can save themselves a lot of time detailing by Showing Dimensions and then Edit > Cleanup Dimensions. You can also create drawings templates that place your saved views on a drawing, show your dimensions (as well as notes, balloons, cross sections, etc.), fill in tables, and clean up your dimensions. These can be immense time savers.

 

[rcamp]

jabbadeus said:





For a single or handful of dimensions, this is true. But for a part with more than a couple dozen dimensions, a person can save themselves a lot of time detailing by Showing Dimensions and then Edit > Cleanup Dimensions.





That is true, I wasn't thinking of the fact that you can show many dimensions at once. However, you often have to do more than just a global cleanup, you often have to switch views.



But my main contention is still:



Only part feature dimensions can be shown in a part model drawing, what you gain in being able to show dim's you more than give up by not utilizing the power of assembly level modeling.



Another issue as far as attempting to show dimensions to meet manufacturing needs is this:



The person milling wants his dimensions to reference one feature, while the person grinding wants them to reference another, and the person on EDM yet another. (This is really what I have to deal with). Well more than one of them are just going to have to get out calculator and pencil and use their head, so your better of just to dimension with function/tolerance in mind. Unless there are one-process-manufactured parts, you not going to be able to accomplish much.



This is why we rely so heavily on CNC. CNC's with good programmers and tech's can put it where you need it well within tolerances, all by just referencing the 3D model. Unless its finished by drilling, the tolerance is +/- .0005. Hit it.



Moldmaking is a unique process, but we can all learn things from each others fields, that's why I'm tossing the ideas out for discussion.

 

[dougr]

The person milling wants his dimensions to reference one feature, while the person grinding wants them to reference another, and the person on EDM yet another.



Manufacturing can make parts any way they see fit as long as the parts conform to my drawing at the end of the day.



My department (Engineering) only makes inspection drawings.



I've never worked in mold making but I have stacks of experience with castings. In some cases castings can have leadtimes up to 18 months so we use a preliminary release process whereby we can release models only for tooling. However, to production release parts a fully released drawing is required at the end of the day.

 

[rcamp]

dougr, die cast dies are very similar to injection molds mechanically. The runners are gates are more complex for dcd's because of the difference between the flow of melted plastic and the flow of molten aluminum and the forces are much more stressful.



But that is a similar situation, it sounds like: the toolbuilder has spent 10's of 1000's of dollars and 100's of manhours cutting the part features in steel before they ever see a drawing. By the time the die goes is ready for production the mold is, a major aspect of the part production cyle is completed, even though the actual production cycle is only just beginning.



I think you're approach is more reasonable, but I do agree the manufacturing process has to be considered in the design of the model/product/component, but it doesn't need to be a consideration in the making of the drawing/print.



Product designers and product manufacturers definitely need to work more closely in the DESIGN stage.

 

[dougr]

It seems to me there are some little understood fundamental issues in this thread:



1) Engineering only puts out inspection drawings (or they should be doing so).



2) Note that GD&T is a function based approach (not manufacturing) to Dimensioning and Tolerancing.



3) Engineering is responsible for fit, form & function first and foremost - manufacturing next, this is the natural order.



Think about it - what is there if parts don't function ?? Nothing, nada, zilch, zero, empty space - function has to come first.



4) It was stated in this thread that:



A dimensioning scheme should reflect how one wants to control a model, not how one wants to detail it.



A dimensioning scheme should reflect the Engineer's design intent for the real part - not just to suit a bloody Pro/E model !!!



This is what's reflected on drawings and should be reflected in models too.



5) As an Engineering Manager having one dimensioning scheme in one place (model) and a different scheme in another (drawing) doesn't do it for me - I want consistency and I want everything per my Engineer's design intent.



Until this practice changes there will always be a need for drawings.



6) As an Engineering Manager my requirement is to fully communicate our design intent so that product will function as intended and be manufactured in the most economical and timely manner (and in that order) - I'm not bothered if it's by model or drawing as long as the documentation is correct and proper release process is used.



However, if it's by model only then the dimensioning and tolerancing schemes IN THE MODEL had better be in accordance with my Engineer's design intent.



7) There are 3 basic types of dimensions in Pro/E:



Driving (Shown)

Driven

Draft



Driven and draft can only exist in drawings.



Driven dims will update with model changes but can lose references easily so should be minimized. Use as a last resort or for reference dims only.



Draft dims are between draft entities and should be heavily discouraged.



8) wtf is a drawing-centric or model-centric organization ???



My organization is product-centric.

 

[dougr]

The attached file is an interesting and pertinent article to this thread.



Of particular note are:



Drafting practices developed over decades standardize how information should be displayed on drawings to avoid ambiguity. No such standards have existed for annotating CAD solid models, and as a result, every designer approaches the task differently.





I'd add to this that I see no reason as to why we can't be annotating models today, particularly regarding dimensioning and tolerancing. It does, however, mean setting up the appropriate dimensioning schemes in model features.





As long as drawings and CAD models are separate documents, however, the temptation will be to treat drawings and CAD models as separate entities instead of parts of a unified product data set.





Also, ASME Y14.5 is a Dimensioning and Tolerancing standard and as such isn't exclusive to drawings. It can be applied to CAD models with equal effect...

 

[rcamp]

dougr, I think that is a good concept, and probably an achievable one, if the software developers will adopt it. For instance, (again) PTC needs to address the issue of assembly level features in using the dim/tol paradigm. You will have to be able to create those draft items in 3D seperately from the feature itself if they are assembly features, unless they can find a way to transmit that data automatically to the part at the part level. This they probably will not do. Hte reason I think they won't is because I have contacted them several times and submitted enhacement requests over 4 years on the issue that in ProNC you can only auto-drill on hole features or axes in a part. I think that precludes assembly features, except with the axes, you can come back and manually created the needed axes on the cylindrical surfaces (extra work!).



I think a better 3D dimensioning/tolerancing paradigm would be a meta-data type concept, where the tolerance is based on what the feature is and the part feature (ie. the assembly feature when queried at the part level) inherits tolerances from the assembly-level feature that created it. Eg., this is a bolt hole feature, therefore the tolerance for body_dia is ***, for c'bore depth is ***.



That is generally how we handle our tolerances. The programmer or moldmaker knows the function of the feature, and determines from that what his tolerances are.

 

[fhodshon]

GMP to me means one thing:



MODEL FLEXING.



if your model ain't a flexin', then its got me a vexin'!



f

 

[dougr]

MODEL FLEXING



?????

 

[kvision]

Model Flexing is the idea that you can change dimensions and the model updates correctly without failure. So changing a fillet radius doesn't crash your model. A good model is robust and flexible. This generally requires a lot of forthought and relations and good sketch setup.