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 ?
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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' www.h2omarkdesign.com
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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.
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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.
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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'
TOP wrote:

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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?
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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
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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
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Hello SMA.
"You are a tool designer and ACAD is still the best all around tool for that type of work. "... You're either a real good salesman, or the first authority I've read who speaks the truth. If you listed all the engineering disciplines by order that they benefited from 3d, dies would be at the bottom.
"1) SW can very accurately unfold a part a bend at a time" ... Individual bend control. What better way to play with form progressions, eh. Although I found out bends only go from folded to flat. Occasionally need incremental bending (flat to 45 to 90)
"2) .... Very important. With featureworks, you can make dumb models fully parametric with relative ease."... I'm looking forward to that. So often have to remove a fillet to extrude a toolbody too. But dose it really work? I have many problems with imported geometry in IV. Often parts get translated a couple of times before I get it. The 3d world is a solid mess it seems. I'm hoping parasolids long history makes it a better translator. Until/if the world unifies on one kernel, dumb solid tools are very appealing.
"3) The configured part can be patterned and used as the basis for your 2D strip design."... you betcha. Number one desire. Even if I design in 2d, want the strip in 3d. So often in design reviews people have no ideal what they are looking at and prevents them from giving good input. With a 3d iso, my grandma can tell what's going on. But the big question, do station configs actually work. Well SMA has said all the right things to support his knowledge of dies. If he says it dose, I'll take his word as the voice of authority.
"ideally you want pre & post operation, so you can overlap parts with different configs to achieve this."... in 2d I show strip in pre-hit position. In 3d you have to show post-hit. But in 3d, easy to add another strip and feed it one station. At least for checking. I've even assembled 2 strips, one progression apart, then boolean subtract and you get the pre-hit remnant and slugs too!
"4)... - great for quoting." ... I never thought of that. a dummy die controlled with a few parameters you can instantly get weights/cost from. Excellent! Combine that with featureworks to deconstruct a part into stations, and a strip template ready made to accept the station configs. You could have a real good picture in no time. I wonder if that's how QuickQuote (quickpress) works?
"5) Variational details that you do over and over "... dies certainly could make use of a 3d library. A lot of planning to preset parameter for bom though. I believe you can specify which sketch dimensions can be used in the drawing at the part level, for auto dimensioning on the print... A way to facilitate detailing of the library part. What would be best, if individual detail drawings of library parts could be ready-made, then pasted into a sheet. I would guess this is not possible, in any package.
"6) Full blown die design on SW is absolutely clunky." ... telling it like it is instills more confidence than a big surprised later.
"Dealing with fasteners is a pain, all the parametric fudging"... Oh no, I'm getting scared, care to elaborate? I know screws are a pita, what parameter fudging? I've heard params in SW are not as good as IV, which seem very easy.
"and frankly the drafting is somehow not clean"...One advantage IV has, I think, is the drawing side. Given all that it is doing, quite fast. And prints are clean and nice as they get. Makes a tough decision. Do you want to be with a pretty girl, or hang with your buddies. Know what I mean???
"it's tough to get a "simplified" side view" ... no different in IV. Big advantage to 2d. I'm thinking of having a generic side of lifters and punch lengths and such. Then section just the unique stuff on the tool.
"Nesting for a stick punch layout for wire EDM? Forget it!"... lol
HEY BIG QUESTION... Sw has ordinate dimensioning??? Anyone written auto-ordinate programs?
"7) Large drawing sets"... I know. Last job I detailed 4 stage tools in one 2d drawing complete. Must have been 40 sheets crammed with details. + plans, boms, order sheets... all in one 8 meg file. They don't update, details might not match the plans, but you can zoom to any detail in a second. In 3d you spend 30% of the last half of design waiting on files to open. Can SW have 10 sheets in one file? Does that one file take forever to open? One print per detail would be slick for end customer, but try to run that through a shop.
"8) On the upside if you want to do full 3D designs, there is no CNC prep"... well a lot of times you have to close up holes and pockets to single point machine. Another + for configs, a "designed" and "CNC" config.
"I have used 3D at times to develop a complex forming operation" ... I've said it many times, 3d makes the hard stuff easy, and the easy stuff hard.
"DISCLAIMER:" ... I have designed dies for 17 years now. Probably 400 - 500 designs, not little ones either. Designed first 3d die with acad r10 (for money, not play), been designing or supplementing design with a parametric modeler for 4 years... outside of SW specifics which I have no knowledge of, I agree with everything SMA has said.
But we're not giving up yet. Are we?
Thank you SMA.
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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.
--

- John

John Eric Voltin
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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

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I stand corrected.
--

- John

John Eric Voltin
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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?
--

- John

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

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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.
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snipped-for-privacy@yahoo.com says...

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
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I hear you Matt. When I saw sketch blocks the first thing I thought about was sketching a whole die with the blocks. I've read others talk about using split method, so I started there.
There are a couple of die specific add-ons. Twice the cost of SW though. Now we're talking close to the price of UG's die package, which I hear is killer.
I may take your advice. Thanks.
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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.
--

- John

John Eric Voltin
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? #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?
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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.
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