Modelling a Zalman Heat Sink in Pro-E Wildfire

i initially modelled this in Solidworks, and it went pretty well. Not
a perfect replica, but good enough for the task at hand.
then i tried to "do it in pro-e". (i'm new at both s'Works and pro-E.)
anyway, after scratching my head, i'm left thinking, "how do you model
this thing in pro-e" ??
i put some of the images online in a simple web page at
formatting link

with screen dumps from solidworks, pro-e, and one-space designer.
could someone help me in my pro-e education by describing the "right
way" to model this geometry in pro-E ?
thanks !
wwswimming
PS a zalman heatsink is one of the best-performing heat sinks among
the hundreds of different fan/heat sink solutions that are available in
the PC marketplace. i bought one - and then i tried to model it in
solidworks. and now i'm trying to learn pro-e !
Reply to
wwswimming
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First thing I notice is patterns, Pro/e is aces at patterns and you get trained in making/recognizing them in solid modelling. SW is the same way, I can't even imagine you'd do this in SW without some patterns. Two, in particular, strike the eye: a linear pattern of the root fins; also, a circular pattern of the radial fins. Then it gets more complicated because these two patterns meet. In solid modelling, it's nice. You don't have to figure out that meeting place ahead of time, they just meet where they meet. With solid protrusions, that's not easy; with surfaces and merging surfaces, it's a breeze. (Maybe what you need is 'thin' surfaces.) Also, another feature of these patterned elements that suit solid modellers (and I can't believe you didn't do this in SW) is mirroring or copying a pattterned feature, in this case, patten a quarter, mirror to produce half and mirror again to the other side. Yes, efficiency features like this is what Pro/e solid modelling is all about, and it has been for 15-20 years. Those other guys are the newcomers, and they just CLAIM it's easy. While they also claim their programs are intuitive and you can 'get the hang of it' with a couple of free tutorials (big, Big, BIG selling point), and you won't have to spend any money on training, you'll wind up staying in 'school' forever, going to comp.cad.solidworks for everything you should have learned in a well-stuctured, step-wise training program. But, because SW hasn't even IMAGINED such a thing (and they've left it to the VARs to do all such 'cleanup' tasks), training, and so the acknowledged need for it in SW, is negligible. So, SW people live this mythology that it's easy. To the contrary, there are training classes and a well-developed, PTC-authored program, through schools/universities, to train people in Pro/e. So, little false hope is created that designing well and effectively can be done without such training.
Locate such a program and enroll. Admit it: you need it!
David Janes
Reply to
David Janes
so can anyone outline/ describe in 3, 4, 5 or however many steps, how to create the wireframes for the solids of extrusion & revolution, using pro-e ?
actually, the quarter pattern was mirrored and then mirrored again to get some "working solids" in sWorks.
Reply to
wwswimming
start by extruding the first fin at the end as "thin" extrusion (far right icons in the extrude menu). Sketch it off the center plane the correct amount as two straight lines with a small fillet. You need to dimension the angle and the length of the large segment from the small segment, not the datums. Then do a two dimension pattern selecting the x axis offset dim as the first, which will be the matl thkness, and sel the angle as the second, using the ctrl key, and enter whatever angle the fin changes by. Do enough to make your first quadrant. then mirror; use the . The mirror again to get all the fins, then a revolved cut around the z axis to get the correct fin shape. 10 minutes.
-jk
Reply to
jk
I made this at work today and it's easier if you do the 2 dimensions pattern to cover half the fins, instead of a quadrant.
A revolved cut, as I said before, won't give the correct geometry so instead, pick the plane of the first fin and extrude a cut on this using the bottom datum plane as one sketching reference and the outer edge of the fin as the other dimensioning reference. Extrude blind depth using the material thickness. After that, highlight this cut feature in the model tree, press the pattern icon and pattern by reference. Then mirror all, put your hole in the middle and your done.
When you sketch the very first feature, which is a thin feature, you need to press the "thicken sketch" or thin feature button before you sketch or you will get a "section must be closed" error in the sketcher.
-jk
Reply to
jk
formatting link
the URL for the almost finished model. the screen flickers a lot when i'm drawing a line at .4 degrees from vertical, so i gave up on the related fin.
i also took a shot at it in one space designer
formatting link
thanks for the help !
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i'll try asking the question here - i wanted to model it as 40 separate solids. when i went to do the "thin extrude", basically creating the exterior fin using a vertical line about a half inch high and a horiz. line about 2 inches long (in mm), the new solid was "stuck" to the old solid.
my original intent was to model them as discrete solids, so i did more wireframe/ sketch mode work to create 2 parts representing 2 sets of fins 4.7 degrees apart. then joined them in the next assembly for a model that's good enough for the next level assembly, the "where used."
is it possible to model the part in "thin extrude" mode, and not get the solid bodies "stuck" to each other ?
another way of asking - if i want to model each fin as an individual solid body, is there a way to do it in thin extrude mode ?
thanks !
Reply to
wwswimming
I use r2001, but a method that should work in WF as well would be.
Model one fin as a 2 side protrusion, your basic fin profile.Reference off an axis I have these already in my start part.
Then create an assembly with default datums and centerline, I have this already in my start part assy too
Then create a datum though cl and at a angle to another datum, defaults will work you can change later, pattern the datum, again it doesn't matter how many times or the angle , you need at least one extra
hide the patterned datum, just to make it easier to assembly your one fin
Assemble the fin to that angled datum the one you patterned, use the center plane of the fin and the plane of the cl of the fin and cl of assy. and then bottom datum. You will be fully constrained.
now component >pattern>select the fin and type of pattern is reference adjust angle and number to fit your needs
Reply to
piearesquared2
That would be assemble to datum you patterned from , not one of the ones that are patterned what's that proe term for the lead object? :-)
You need to drop something in the assembly prior to this so you can mirror and copy the fins otherwise you will get error First assembly component can not be moved or copied at least in r2001
Make sense otherwise??.. You can use BOM to get count of fins, I think
Reply to
piearesquared2
Might of steered you wrong a little , it will do what you need, BOM is not going to return the proper values as you will need to make a assembly cut to get rid of the fins you want and they will still appear on the BOM
It's been a learning experience for me too :-)
Reply to
piearesquared2

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