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

http://www.geocities.com/wwswimming/

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 !

 

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

 

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.

 

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 <edit><features
operations> <copy><mirror all>. 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

 

thanks very much, printing out your instructions now to use on the
other machine.

 

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

 

http://www.geocities.com/wwswimming/zalman_pro-E2__.jpg

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

http://www.geocities.com/wwswimming/zalman_OSD2__.jpg

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 !

 

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

 

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

 

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

 

oops after looking at your jpegs I'm way off base....sorry