Should I buy SOLIDWORKS?

Should I buy SOLIDWORKS?

Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.

1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.

2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.

3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg

4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?

5 - Is there window selection in sketch environment? in model? In
drawing ?

 

Diemaker, I can't say I understand your first question -- maybe someone
else will answer. But for the 2nd thru 5th questions, here are my
thoughts:

2) Performance is generally pretty good on machines which have some
power. Sending an eDrawing of a large assembly to someone with a
typical laptop/notebook computer is likely to result in some frustration
for the recipient. Size of the eDrawing can vary greatly. Complex
geometry (especially some things like helical sweeps which would be
needed for threads on screws or springs, if you have either) will
greatly increase the file size. I would expect an eDrawing with 200
unique parts and 500 total to be somewhere between 5 and 10 megabytes,
but it could be larger depending on configurations and complexity of
parts (as mentioned above). Also, if you have to embed the code for
viewing the eDrawing (making it a self-contained executable) it
increases the file size significantly, although not enormously. Have
the recipient download and install the eDrawings Viewer and you won't
have that problem.

3) Yes, SolidWorks has the analagous functionality in its drawing
package. Pretty easy to use and very flexible, once you get the hang of
it.

4) Don't believe you can turn layers on and off in import from DWG or
DXF, but you can handle that pretty easily by just making WBLOCKs of the
data you really do want. SolidWorks, like Inventor, generates drawings
from the 3D model, not the other way around, so typically what you want
to do with a DWG or DXF import is to create a PART, not a DRAWING
sketch. In so doing, layers are irrelevant. In making drawings (not
parts or assemblies) layers CAN be created for different type entities,
like dimensions, text and title block format lines. That's mostly
useful for exporting back out to DWG or DXF formats, for whatever
purpose you do that. For example, just like with AutoCAD naturally
sometimes you want to export just the object lines for use with CNC, and
so you want to be able to turn all the other layers off. You can do
that.

5) Yes, selection "windows" in all three environments work pretty much
just like AutoCAD. Drag from left to right and it's an include window,
right to left is a crossing window. SolidWorks doesn't have the other
fancier fence type selection methods or the type of filter selection
methods that AutoCAD has, but it does have a "Selection Filter" toolbar
which allows you to selectively filter such kinds of entities as Faces,
Edges, Vertices, Dimensions, Sketch Segments, Centerlines, Planes,
Datums, Weld Symbols, etc., etc..

'Sporky'
www.h2omarkdesign.com

 

I'd say all 5 are possible without too much difficulty. The drawing in
3 is not difficult at all but you might have to use a trick. 4 is not a
problem. 2D to 3D tools and dwg import will let you select layers and
fix up poorly drawn ACAD files. There is window selection though I dare
say this aspect may be used differently in SW.

I am not a big fan of edrawings. But others here are. You can section
and measure or not depending on how the file is saved.

If I understand 1 that would not be too difficult.

Now if you are well experienced in ACAD you may find crossing over to a
feature based parametric modeler a challenge. If you can forget ACAD
and approach SW with an open mind you will pick it up quickly.

 

I stand corrected on #4 as far as selecting layers on import goes. Paul
is right about that, now that I think back on it (haven't done it in a
while). The rest of what I said should be valid.

'Sporky'

 

Not quite true. You can have overlapping or touching sketches and extrude
separate bodies from them. The key is to use the contour selection tool to
pick the appropriate entities. If you uncheck the Merge box, then they
remain separate bodies.

WT

 

? #1.... I've also used a master sketch in the assm to control multiple
retainers and trim steels. Change sizes in one sketch and it rebuilds
all the individual part files. Layout drawings in general are no
problem at all.

What part of the country are you located in if you don't mind me asking?

 

Diemaker,
I am one of that "handful" of 3D die designers and I have sent a edrawings
proffesional file to your email, along with some comments. Take a
look. ------------I just looked at the file I sent, and I forgot to enable
the measure function. I will send a new file.

Good luck
Mike Eckstein
Tool Engineering Systems

 

No, what I did was 3 separate extrudes, each one picking its own contour.
Sorry if I mislead you.

WT

 

Good Edrawing info. The size is what I was hoping for. I believe SW
users get access to SW secure server for FTP of large files??? I
pictured the self-contained executable increasing the file by a
consistent size. Is this not so?

self-contained executable is a big plus since I would use edrawing
mostly for 3d design reviews with project managers, usually PM's have
broad band, but IT don't like special programs. And PM's don't
like updating software.

Scanning the board, seems some have problems with edrawing prints. But
models are reliable. I suppose there are all kinds of thing you can
draw on a print that might go wacky in an edrawing, Where as a model,
although complex, is consistent to translate. Does that rational sound
right? Things that go wack in an edrawing print are user blocks,
symbols, special tolerance or fancy fonts. The geometry, simple text
and dims are stable.

I could see edrawings a base for a paperless shop.

 

Thanks for reply, I do want this info. I've studied IV for 4 years.
Done real work with it. I know the differences/limitations of 3d. And
frankly, I see laying out tools in 2d then importing to 3d. 2d is
fluid, much easier to move a cut from one block to another. Much easier
to copy a portion of the design up 50" and draw in a different ideal,
then trash that ideal and move back the original. Dies are mostly flat
plates with openings and inserts that have to be arranged, 2d works
best for this. Call me stuck in my ways, but unless things in SW are
really different, I will still be using acad... And what could be
really different in SW is the configs. So I will belabor this.

Here is an example for question #1.
http://img326.imageshack.us/img326/7735/splitpart1zk.jpg

Can that one sketch be extruded, then split into the 7 different
blocks? Each block being a "config" that will be a separate item in
the BOM. I'm not familiar with "part configs" or the split
feature, so please be basic. You see #4 is gapped, or disjointed. Can
that still be split? #1,2,3 touch, but not with a straight line. Can a
split zig-zig and terminate? #5 &6 would be separate inserts inside
holes in #1. I made one rectangle and the other round corner to
complicate it. #7 is a block on top of another.

This duplicates what I call "master sketching" in IV. I create a
part file of just sketches, then derive into separate parts for
extruding. Change the master, the blocks change. Configs seem to make
this master sketching possible within one file. Maybe split isn't the
right approach, instead extrude the parts individually and make
configs. But the goal is to create multiple parts in one file that will
individually BOM and detail. So am I right on, asking for trouble or
completely dreaming?

 

Rory: Chicago. Sounds like you know what I'm talking about. Weaving
plates around each other, adjusting them as the design progresses or
revision hits. 2D die designers will always talk about how you can't
"stretch" in 3d. Master sketching is a way to achieve this.

 

In IV you can "dice up" a sketch and pick about any individual
region(s) to extrude. Regions can be coincident, butt or over lap. SW
needs a special command for this? Maybe were thinking the different. I
have an picture in response to TOP.

 

Having trouble posting, Diemaker -- I'll see if I can get a message
through to you directly.

'Sporky'

 

SW can't make separate bodies out of sketches that intersect or touch at
an edge unless you do it in multiple features. SW can do as you say
with dicing up a sketch, but this is typically seen as not an incredibly
stable way of doing things. Personally, I think SW added it just so IV
couldn't say that they did something that SW did, not because it was a
great idea.

No one has mentioned the new SW06 sketch blocks functionality, where you
sketch in an assembly and make parts directly from the assembly sketch.
I think this is far better than using contours in the parts and
splitting the part and then reassembling an assembly. There are too
many advantages to assemblies and too many disadvantages of multi-body
parts and contours.

There are also things like part templates that could be used, and a
technique using copied assemblies with parts already in them.

In fact, general tooling dies are not that different from molds that you
couldn't use a nice mold program like Moldworks to automate things quite
a bit.

I'd encourage you to step out of your autodesk world and try some
different approaches.

Matt

 

Howdy,

Ok. Right up front: I don't know a lot about CAD, a smattering here and there.
I know a lot more about CAD than I know about the intricacies of strip or
progressive die design. Metal forming is not totally foreign. The automation
and strip development are the interesting, and totally foreign, parts to me.

I think you might be going about your quest in the wrong way. You have
developed, over the years, methods that are presumably highly productive using a
certain set of software tools. You'd like to adapt these methods so you can use
a different, more comprehensive set of tools to extend your capabilities or
somehow improve on what is. That's where I think the problem lies; trying to
adapt methods that rely on the strengths of one (or a set of) program(s) to
another program that has different strengths (as yet undefined, comprehended,
even imagined?). Doing this you end up focusing on details that are probably
irrelevant. No offense meant, but getting wrapped around the axle about whether
or not a program can pick discrete regions, or boolean them on the fly, out of a
single sketch is not going to be productive. I also think that (what I imagine)
you're intended usage of configs, or table parts, is going to be a dead end,
that other methods will prove to be more effective. The actual "strip" part may
be another story; good use of a config type entity. I also would forget most of
what IV's pseudo-skeleton modeling leads to. It's a really pale imitation of
what's possible using other (loosely related; it's all related, e.g. xref stuff)
methods of creating dependencies with another software (any of several programs,
SW, SE, Pro/E, if I were to guess).

I don't know for a fact that any single 3D software will compete favorably with
your well developed integration of 2D / 3D methods. You are not alone in that
respect. I sometimes work in a field (general aviation) that still relies
heavily on 2D. In part this is because mid-range 3D is still assimilating high
end trickle down (strictly speaking; 3D, certainly "mechanical" is not
emerging -- it's old stuff) and, like you, a lot of people still get the job
done faster using 2D than they can using strictly parametric 3D. Fact or
perception? I don't know. It's something I struggle with myself. Sometimes
it's a toss up, an extension of the napkin sketch vs. engineering drawing
debate. Hand drawn sketches are still, undebatably, the best way to define and
communicate some simple structural repair and that's what goes into the
engineering documentation and is submitted for reigning authority (FAA, DER)
approvals. Sorry, meandering. That's a given; the "design" happens in the
head. Drawings are just documentation and communication of the abstracts. Here
we should be just as interested in how the software can aid the "in the head"
processes and communicate what 2D doesn't lend itself to; 3D shapes and
contours.

I don't really know how one might better (?) go about it. Knowledge of both
software (well beyond "basics" and a tentative grasp of "advanced" topics) and
application is obviously necessary. Perhaps partner with someone to fill in the
missing pieces, someone having intimate knowledge of any given program's
strengths. With the pooled knowledge working scenarios can be explored and
evaluated to see how they stack up against your existing methods. Considerable
investment will be required of both parties. You might also check some of the
local trade / tech schools, colleges, etc. Chicago should be a fertile area for
that; something to be gleaned or maybe a deal to be struck (what can you teach
them?).

Do wish you luck with it ...

 

Thanks Michael. That's a terrific edrawing. A mold, not a die, but
certainly comparable in complexity if not more. Lots of holes. Lot of
model for 4 meg self contained file. Amazing. It was jerky, and I got a
pretty good machine. Love the configs. Super. Can the configs include
different positions? Really want to be able to click a button and show
open and closed. Edrawings personify the philosophical differences
between SW and adsk. DWF is stylish to the point of obscurity. Edrawing
is like Chryslers big buttons you can operate with mittens on. I just
don't have any problems operating edrawings.

 

Hi there - absolutely correct. You are a tool designer and ACAD is
still the best all around tool for that type of work.

<<what follows are _my personal opinions_>>

2d kicks the ass off of 3d for full tool design, however consider the
following:

1) You need to do an accurate development and SW (or 3D) is exceptional
at doing this. SW can very accurately unfold a part a bend at a time
and your config list can show you your bend sequence. You must have
this. 2D blank development is just a waste of time and not as
reliable.

2) You most likely work with customer supplied models and you can use
their models to develop your flats. Very important. With
featureworks, you can make dumb models fully parametric with relative
ease.

3) The configured part can be patterned and used as the basis for your
2D strip design. You can take all your side views off of the patterned
part model. You insert a part into an assembly and then pattern it to
your advance. The only issue here is that the part can only be one
configuration per station - ideally you want pre & post operation, so
you can overlap parts with different configs to achieve this.

4) Parametrics allow you to make a progressive die "shell" with much of
the right stuff in the right place. I developed a model that I used to
generate a properly timed side view of the stripper, pilot-perf and
first two pilots on the correct advance and properly sized - including
upper & lower shoe thickness, parallels, die, punch plate, stripper
guide pins . . . The timing was also done. From the top view, I was
able to manipulate mounting slots and handling holes, change the
guidepin style and so on. This allowed me to play with options rapidly
without any drafting needed. It saved at least 8 hours a job and it
gave me a great "main" side view. I also developed the same for
compounds and this could do a basic design shell and project your
material costs - great for quoting and so on all with a designed shell
as an output.

5) Variational details that you do over and over again but only at
different lengths, sizes etc. are really great to do with SW. We used
to do a unique type of self releasing form punch (i.e. no ejection, sky
hooks, etc) - the same old design but a slightly new length - save
yourself an hour each time you generate a fully dimensioned detail.

6) Full blown die design on SW is absolutely clunky. Dealing with
fasteners is a pain, all the parametric "fudging" and frankly the
drafting is somehow not "clean". Layering is weak, dimensioning a pain
and strip layout a nightmare (not too easy to make a concise strip with
all those needed "real life" elements - scallop cuts, 45 degree
cut-bys, tolerance split for mismatch and so on). There are just too
many encumberances to doing a full design with this product in a timely
fashion (remember - my opinion only) - it's tough to get a "simplified"
side view - my theory has always been to "tell a story" showing just
what the toolmaker needs - the "high fidelity" views that SW gives are
too cluttered to tell a good story - a good side view can be had, but
sometimes you need more views to "tell the story" adequately. Nesting
for a stick punch layout for wire EDM? Forget it!

7) Large drawing sets and the need to split your drawings into separate
documents is a barrier to sharing data between your drawing panels.
Not impossible, but another encumbrance. I'm personally used to a
single sheet "monolithic" drawing with many frames scaled up or down as
needed. Exchange of data between sheets is easier with raw 2D - easier
to "cheat" which is sometimes needed.

8) On the upside if you want to do full 3D designs, there is no CNC
prep down he road and your data integrity is absolutely awesome. This
is the upside and you can easily see the relationships between
components. In come cases, this is better, sometimes worse. With 2D I
like to do a superimposed design with layering viewed thru the upper. I
can see all of the design at a glance and use layers to see different
states of the design. 3D can do this as well, but sometimes not as
easy to see things. I have used 3D at times to develop a complex
forming operation - good for visualizing a design. In one case, I had
a 3 sided form op that clasped to the upper (classic - formed around
the upper, never to be removed), so I needed to design a form punch
with the ends that moved out on the downstroke and released on the
return stroke - the good news - the part sat on the lower pad and did
not clasp the punch - 3D helped a lot there - but the base design was
still 2D.

9) Libraries can help in either realm. Developing a good 3D library
takes time and will make 3D design easier. Most likely, you have a
good 2D library that is already saving you time. Personally I find
this to be the thing that I miss the most in 3D design (tooling
specific). Maybe that's one of the reasons that it is "clunky" for me.

DISCLAIMER: The preceding is simply one person's opinion and this
being offered does not preclude others from doing it better or having
great success with pure 3D tool design.

For me, your original statement about the economy of 2D design (for
this type of work) rings very true.

Later,

SMA

 

Sean,

I found your discourse very interesting and appreciate you taking the
time. I guess I could sum it up by saying that in many industries a lot
of information is carried in the head, not on the paper. Tool and Die
and mold making are two such industries. I have no idea what half of
your terminology means. What is important is that you and the readers
of your prints know the conventions. 3D simply doesn't lend itself to
some of the shortcuts that account for this kind of skilled knowledge.
It almost sounds like your drawings are more symbols with dimensions
than an attempt to detail every little feature.

On the other hand, you have a very efficient system setup in 2D. No
doubt it is fast for you. The real question then is, can 3D be setup to
be as efficient. You speak of using layers. Layers are indeed a
powerful tool in 2D and in some 3D programs like UG. The question in 3D
is whether layers are needed at all. It can come down to a difference
of methods.

I have to agree about drawings. SW could be a very fast drafting
package if they had thought to use the sketcher to make scaled 2D
drawings in the draft module. The fact is, you can't take the hard
stuff that needs 3D treatment, drop it into a drawing and then finish
up with 2D to complete the drawing. It is just outside a 3D system's
ken. But that would sure speed things up. SolidEdge has tried to do
this but still comes up short.

TOP

 

Hey Jeff... I kind of feel like I've just been thorough therapy. Hehe

My 3d mentality is changing. Every now and then I get a moment of
clarity and a little more light sheds on the darkness. I do have a lot
of baggage, but there are many treasures in those bags.

I feel I'm a trailblazer. I did not grow up in automotive country
where 3d is highly sought, I grew up in electronicville, where we mass
great quantities of little details. And none of my cronies have made
much effort to explore 3d. One of the better independents I keep
contact with is getting more crushed parts, as am I, and he's paying
a proe jock to do his extrusions. Last time I out-sourced was 3+ years
ago, and wouldn't think of sending that job out today. Search the
groups, you see some die interest, but not much proof of action.
That's what I see, seems everyone has 3d, but not using it. Talking
prog dies of course.

I had three designers under 28 years old. You'd think they would be
gun ho on 3d, but no. They would say...3d? yeah, I can do that, give me
another die to design. My oldest designer however went to SW classes
after a 10 hour day. 4 years later though, they still use acad.

Find a partner? That's what I've been doing. I got my best dress
and good perfume on waiting for someone to buy me a drink. Hehe. As far
as schooling, would you really want ME in your class? Innovation
doesn't come from a procedure book, it comes from expectations and a
will to overcome. I have at least 1.5 of those things.

There was a well known designer (in our circle) that was famous for
sketching as he talked. When I finally met him at a tool review, sure
enough, he penciled the most perfect little iso drawings all over that
print. It was like watching Charles Schulz draw snoopy. I'll never
forget that.

I didn't obsess about regions, they did. I want to know about part
configs.

Thanks for the encouragement, if I get SW I'll let you know how it
stacks up. In fact, I'll let everyone know. Hehe.

BTW, I wonder what grade Roxanne got on your "challenging implant"
model?

 

I'm assuming you mean open "like a book" so you can see both halves at the
same time. It can be done, I think the easiest way would be make a new blank
assembly and add in the original assembly of the mold (or casting die)twice.
Use the properties function to change the configuration of one half or the
other in the new assembly to what you need. Then make your edrawing. As you
will find out there are a lot of ways to skin a horse. This is just one of
them.
Also that file, it was not at all jerky for me. It could be your video card,
if you decide to get SWX check the website for recommended cards. It will
save lots of grief down the road. Give me a call if you have any questions.

Mike Eckstein