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:
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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 ?
Reply to
Diemaker
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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'
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Reply to
Sporkman
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.
Reply to
TOP
The followup postings have answered most of your questions, but didn't mention one detail regarding question 1. You can create a single part in SolidWorks that contains four separate rectangles that are extruded to form four separate bodies. Unfortunately, SolidWorks will not allow these four rectangles to be butting together as you mention. Inventor will allow rectangles to be butting and still extrude, but SolidWorks will not. Any touching or overlap of the rectangles is not allowed in SolidWorks. Otherwise the scenario you propose is possible within SolidWorks. You can produce the desired result, but not with the method you described.
This particular topic is one area where Inventor is clearly superior to SolidWorks. I hope that someday SolidWorks will duplicate this capability since it reduces the need to trim sketches and improves efficiency. I should note that Pro/E also has the ability to extrude touching or overlaping sketch entities.
Reply to
John Eric Voltin
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'
T>
Reply to
Sporkman
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
Reply to
Wayne Tiffany
Apparently, I was mistaken about SolidWorks having this limitation. This morning I received an e-mail informing me of Contour Selection within SolidWorks. While working on a sketch, right click in the graphics area and choose Contour Select Tool. This will allow you to select the contours that are used for the feature including touching or overlapping sketch entities. It works quite nicely and I anticipate using it on a regular basis.
See the help file for complete details.
Reply to
John Eric Voltin
? #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?
Reply to
Rory
I stand corrected.
Reply to
John Eric Voltin
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
Reply to
Michael Eckstein
I have been testing this feature and I have not been able to create separate adjoining bodies with a single extrude using the Contour Selection tool. Merge does not appear to be an option within the context of a single extrude. You can create two separate, adjoining extrusions and uncheck the merge box to make them separate bodies.
Any suggestions?
Reply to
John Eric Voltin
No, what I did was 3 separate extrudes, each one picking its own contour. Sorry if I mislead you.
WT
Reply to
Wayne Tiffany
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.
Reply to
Diemaker
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.
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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?
Reply to
Diemaker
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.
Reply to
Diemaker
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.
Reply to
Diemaker
Having trouble posting, Diemaker -- I'll see if I can get a message through to you directly.
'Sporky'
Reply to
Sporkman
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
Reply to
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 ...
Reply to
Jeff Howard
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.
Reply to
Diemaker

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