Solutions Current Issues > April/May/June 2007 > BENNY & BRUCE
Email LinkHOSE DESIGN
(or, How to Add “Flare” To Your Modeling Projects)
Editor’s note: Our engineers here at RL Hudson use Pro/ENGINEER® solid modeling software to design parts, and we know that many of our customers’ engineering departments also rely on Pro/E®, which is, after all, the standard by which all other modeling programs are judged. With that in mind, we at Solutions have enlisted two Pro/E experts – Benny Foreman and Bruce Sumpter – to share some design insights with our readers. Both Benny and Bruce served as application engineers and independent consultants for PTC (the company that developed Pro/E) prior to joining our engineering department here at RL Hudson.
Benny Foreman graduated from the University of Oklahoma in 1995 with a Bachelor’s Degree in Mechanical Engineering. Since then, he has split his time between working as a manufacturing engineer and as an application engineer designing manufacturing software. Benny has been part of RL Hudson’s engineering team since 2003.
Bruce Sumpter earned a Master’s Degree in Mechanical Engineering from Oklahoma State University in 1985. He now has two decades of experience working with engineering and enterprise-level software solutions. Bruce joined RL Hudson’s engineering team in 2004.
Today’s extra special guest: Dave Johnson, who earned a Bachelor’s Degree in Education from Northeastern State University in December 1991. Dave has 25 years of experience in the manufacturing field, mostly in the tooling trade. He joined the RL Hudson team in 2004.
Gentlemen, take it away…
Hose Variations: Clockwise from upper left, four types of
hose you can create in Pro/E are straight extruded,
revolved with flared end, variable section sweep, and
regular sweep.
Benny: This time we’re looking at various methods to model hose in Pro/E. Depending on the complexity of the hose, there are many ways to approach this. What we’ll discuss today are a few of the most common ways we have seen.
Bruce: To help us out with this, we’ve asked our colleague Dave Johnson to sit in and offer a few insights. Welcome to our humble column, Dave.
Dave: Nice to be here. (slight pause) I was promised sandwiches.
Benny: We were, too. (pause) So, anyway, today we’re going to discuss four progressively complicated types of hose modeling situations. Let’s start with a basic straight hose as our first example. To model a straight hose, simply extrude or revolve the cross-section. Extrusion alone can only produce straight hoses; using the revolve function will allow you to design flared ends.
Bruce: But most of the hose projects we see here at RL Hudson are not that simple.
Menu Sequence: Follow the steps shown above to create
points offset frp, a coordinate system.
Benny: And before we go much further, we should probably introduce a few bits of hose terminology. Hoses are typically measured by a series of arm lengths driven by theoretical sharp points.
Dave: And these points are most easily created offset from a coordinate system.
Bruce: That is, if the location of these points is available to you.
Dave: If they are, you can enter the X-Y-Z coordinates directly into the point table.
Bruce: Just be sure the points follow the “right hand rule” for pluses and minuses, otherwise your hose will end up being the opposite – a mirror image – of what you want.
Benny: If you don’t know the X-Y-Z coordinates, which you probably won’t if you are creating a hose from scratch, then feel free to use any other method to create these points.
Bruce: Once you have points, you can create your hose using the “pipe” feature in Pro/E. Select the points, then enter an O.D., wall thickness, and bend radius. And that’s all you need to do!
Dave: But keep in mind: SAE hoses are generally specified by wall thickness and I.D., so the geometry of the “pipe” feature is not defined by the most important dimensions.
Bruce: You could make a solid pipe and use a shell with a negative value to make it thicken outward.
Benny: But that is definitely not what I would call “best practices.” To overcome this limitation, the next option for hose modeling would be to use what’s called a “sweep.”
Bruce: To use this “sweep” option, first you must define the spine of the hose. To do that, insert a datum curve referencing the theoretical sharp points, then you would typically use a swept thin protrusion.
Benny: So now you have designed a 3-D hose with multiple bend radii. The next step up in difficulty is a 3-D hose with flared ends.
Dave: If the flared section does not intersect a bend, then it is perfectly legitimate to use the sweep option and then cheat by cutting the end of the hose off and adding a revolve feature for the flare.
Benny: Or, you could be more efficient with feature use, and thus impress your friends! Here’s how: When you create the sweep feature, and you’re selecting the trajectory for the sweep, you can trim the ends of the trajectory, then add the revolve.
Bruce: That keeps you from adding geometry, taking it away, and then adding it back again.
Benny: Or essentially “whittling” at the model.
Dave: Don’t be a little whittler, because we belittle whittlers.
Bruce: Nice!
Benny: Finally, if the hose’s flared end goes into a bend, then the only real way to model the geometry correctly is to use a variable section sweep.
Dave: Which is essentially the same as a regular sweep, except that the cross-section can vary along the trajectory.
Benny: Here’s how we prefer to do it: Define the hose’s spine just as before. Using Pro/E, measure the total length of the spine curve, because you’ll need this data later. Then create a graph feature.
Bruce: The graph feature lets you define how the hose’s I.D. changes along the spine.
Dave: That’s relative to the position along the spine.
Benny: So when you are creating this feature, sketcher will come up and then you insert a coordinate system. Then draw the curve defining how the I.D. profile will change along the spine. For instance, a 2” I.D. hose with no flares would just be a straight line at y=2.
Dave: Whereas a hose with a single flared end would have a straight line for the main diameter, then blend up to another straight line representing the enlarged diameter.
Benny: The total length from the coordinate system to the right end of the sketch should be the total length of the spine curve noted earlier.
Bruce: Next, you insert a variable section, thin protrusion (sweep), select the spine curve as the trajectory, and set the I.D. of the cross-section by using a relationship to the graph called “eval graph.”
Dave: As opposed to “evil graph”!
Bruce: Which is never a good idea!
Benny: So, to recap: What “eval graph” does is set the I.D. of the sweep equal to the height from the coordinate system to the curve you sketched in the graph as you move along the spine. To set this relationship, set the I.D. of the sketch in the variable section sweep to evalgraph (“graphname”:trajpar*spinelength) where graphname is the name of the graph feature and spinelength is the measured length of the spine.
Bruce: This is obviously a fairly complicated procedure, so check out this column on the RL Hudson web site for a more detailed explanation of this process.
Benny: Absolutely. The only thing more difficult than this is if the hose cross-section has to change from circular to non-circular in areas to avoid some obstruction in the assembly.
Dave: But we don’t have room here to go into that!
Benny: Nor the patience.
Bruce: So this discussion has been about hose design. To create a first-class hose drawing, be sure see the Tech Session from our July – August – September 2006 issue.
Benny: And shoot us an e-mail if you have other insights into hose design using Pro/E. As always, you can reach us at benny&bruce@rlhudson.com. Pro/E is a fantastic program, so make it work for you!
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