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eobet

Solidworks Challenge: Offset These Surfaces! ;)

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I thought I found a "great new way" (for me at least) to create models which doesn't have a single planar surface in Solidworks. Oh, how wrong I was.

 

The attached model is 100% boundary surfaces and filled surfaces, all built using adjacent edges.

 

One would think they then would knit together perfectly, but they do not.

 

Which means that I can't offset the surfaces together outwards, which I need to be able to do.

 

Apart from modeling surfaces in something called SOLIDworks, anyone know where I went wrong? :)

surfaces.SLDPRT.zip

post-526-1256167854.png

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have you tried, Thicken? ..sometimes it works it forces the extension of the boundary.

the corners seem to be the issue,.. the common vertex is lost when offset outward..

post-5796-1256175367.png

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Apart from modeling surfaces in something called SOLIDworks, anyone know where I went wrong? :)

 

Did a boundary check in NX6 and showed gaps where indicated (yellow) rebuilt the surfaces shown and it knitted and thickened as expected.

Can you tighten up the tolerance in SW, if so try that ?

 

Otherwise get NX :)

post-22000-1256179419.png

 

Cheers

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Guest under-dog

I tried to make sense of it. Very confusing method of building. There were a lot of just odd geometries in there.

 

Much like the couch. I think that was your thread as well. That one I downloaded and was able to get to offset although it took a lot of effort to go back and repair all the sketches and core geometry that was, to put it kindly, a bit of a mess.

 

I think you just need to develope some cleaner methods of developing geometry. Rhino is more forgiving with butchered in geometry. Somewhat forgiving with less than clean geometry. SW is far less forgiving.

 

 

 

Sorry to be so brutal but looking at the files it is what I see. Just saying it is a more of a refinement of process than it is Software issue.

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Did a boundary check in NX6 and showed gaps where indicated (yellow) rebuilt the surfaces shown and it knitted and thickened as expected.

Can you tighten up the tolerance in SW, if so try that ?

 

Otherwise get NX :)

 

Thank you for identifying the problem areas. What is NX?

 

Also, I found no way so far to increase the tolerances (I found options for it in the document settings, but they didn't seem to have any effect... I think they're for measurements only).

 

I tried to make sense of it. Very confusing method of building. There were a lot of just odd geometries in there.

 

Much like the couch. I think that was your thread as well. That one I downloaded and was able to get to offset although it took a lot of effort to go back and repair all the sketches and core geometry that was, to put it kindly, a bit of a mess.

 

I think you just need to develope some cleaner methods of developing geometry. Rhino is more forgiving with butchered in geometry. Somewhat forgiving with less than clean geometry. SW is far less forgiving.

 

Sorry to be so brutal but looking at the files it is what I see. Just saying it is a more of a refinement of process than it is Software issue.

 

Hehe, maybe. The idea was to do a silhouette and extrude it, then cut away where I wanted the next curve to begin, and use that for the next surface, until there was nothing left of the straight surfaces of the original extrude. That way, I didn't need to use 3D sketches or projected curves (though I did use a 3D curve in a few places).

 

To me, though, the fact that SW isn't "forgiving" (in that it cares about how an edge I'm building off of was created) is to me a software issue. :)

 

So, sigh... I guess it's finally time to move away from Solidworks and learn Alias.... *shudder* :(

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Guest Marc UK

For me, there was no need to do all those things....I just rolled back a couple of steps and then tried to check the integrity of the surfaces and joins by adding a Surface Plane to the open side and then try making it a solid (enclosed volume) using the Knit tool. It failed this test, and in doing so showed me which was the problem surface (Surface-Fill#2). This was caused by a dodgy edge which I first healed with the Heal Edge tool, then re-built the surface using Surface Fill...following this i was able to knit and produce a solid from it which then shelled with no trouble at all (see pic). (Therefore, I would say there's nothing wrong with the tolerances in your model ).

 

However, as expected from the rather odd geometry this still produces some offset surfaces that would ideally require re-working manually (note the mismatching covergence points highlighted). Shelling, ofsetting, thickening etc is always invariably done better manually - piecemeal, with any weird geometry anyway if you want decent results that don't upset your workflow downstream...just my opinion though!)

post-11180-1256237682.jpg

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SolidWorks has never been really forgiving,.. at least for me,.. it has ALWAYS been filled with workarounds.

But,.. (and I hate defending SolidWorks) after dissecting your example further,.. if you look at each surface individually,... offset, untrim and extend... you'll see each boundaries extents and the adjacent boundaries trim limits.

Relying on SolidWorks to save you... man,.. you'll be cursing it every day

Part of the workaround game/responsibility of modeling odd shapes is modeling in flexibility for later gotchas. :ohno:

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I too think you've been using edges, for edges, for edges, for edges.

 

Solidworks (like any system) will always lose some tolerance with each build of an edge or surface, unlike some other systems though you can not adjust your tolerance settings and maybe that would make for a nice enhancement request.

 

Working off of edges is perfectly fine, but try to limit the amount of times you do it.

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Guest under-dog
Did a boundary check in NX6 and showed gaps where indicated (yellow) rebuilt the surfaces shown and it knitted and thickened as expected.

Can you tighten up the tolerance in SW, if so try that ?

 

Otherwise get NX :)

 

Thank you for identifying the problem areas. What is NX?

 

Also, I found no way so far to increase the tolerances (I found options for it in the document settings, but they didn't seem to have any effect... I think they're for measurements only).

 

I tried to make sense of it. Very confusing method of building. There were a lot of just odd geometries in there.

 

Much like the couch. I think that was your thread as well. That one I downloaded and was able to get to offset although it took a lot of effort to go back and repair all the sketches and core geometry that was, to put it kindly, a bit of a mess.

 

I think you just need to develope some cleaner methods of developing geometry. Rhino is more forgiving with butchered in geometry. Somewhat forgiving with less than clean geometry. SW is far less forgiving.

 

Sorry to be so brutal but looking at the files it is what I see. Just saying it is a more of a refinement of process than it is Software issue.

 

Hehe, maybe. The idea was to do a silhouette and extrude it, then cut away where I wanted the next curve to begin, and use that for the next surface, until there was nothing left of the straight surfaces of the original extrude. That way, I didn't need to use 3D sketches or projected curves (though I did use a 3D curve in a few places).

 

To me, though, the fact that SW isn't "forgiving" (in that it cares about how an edge I'm building off of was created) is to me a software issue. :)

 

So, sigh... I guess it's finally time to move away from Solidworks and learn Alias.... *shudder* :(

 

You must keep it in context. Yes Solid Works has it flaws like any software. It is what it is. It is a parametric solid modeler. These types of software are typically designed to work simpler less organic forms. This is by no means to say that they can not make very comples forms even of a very organic nature. You just need to really know what you are doing. You need to be able to predict what the software requires, how it wil react especially to changes and so on. This all comes with experience and deeper understanding.

 

There may be some of what might be percieved shortcomings in flexability in some areas but here is a trade off. Parametrics can be the root cause of these "flexability issues" but adds a whole different kind of flexability that you do not get from a WYSYWYG modeller like Rhino. Yes Solid Works cares very much for how something was built and not just the end result. If you know how to set things up properly this can be a huge advantage to making changes downstream. If you do not know what you are doing then you will be creating a complete mess and beating your head against the wall in no time. Strategy is the key.

 

 

I have worked with people's files that were a masterpiece of strategy and I have had files that I have taken a 2 minute look at and knew right a way I was better off to either parasiolid the part out and press on from there or just start the part over becuase the mess that someone created was far more work to even try and navigate let alone make effective and efficient changes.

 

 

With that said I use both SW and Rhino. I use rhino(with Sw as well) to experiment and "feel out" a design. You can slap @#$@#$ in pull twish and bully stuff around to get close to what you want and work through quick iterations. However this type of practice can and often will(especially in the wronge hands) produce something that may "look like" but when studied carefully is a complete abomonation of geometry. Especially for taking to an engineering level. So I use them as frameworks to reconstruct a clean and proper file in SW.

 

You have no idea how many files have been sent my way by someone that did not know how to evaluate what they had recieved from a contractor or vendor. I take a look at then and it is obvios that the files were patched and slapper together. and that the person had no clue what they were doing whether it be SW or Rhino. It is also clear in a lot of cases when someone has jockeyed and manipulated something in Rhino to make some form "tweaks" even though they said they use SW all the way. If they really did it all in SW then they did a really bad job anyway. Otherwise they null and voided the parametrics anyway to import into rhino for tweaks.

 

Dont get me wronge, done right this sort of thing can work out, especially for concept work. But to try and pass it off as an engineering file........shame on them. Shame on the people woho accepted it too.

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Guest kaiza

I haven't looked at the file, but 2010 knit feature gives you adjustments on tolerance - allowing it to knit across bigger gaps.

 

However, even if this worked for your file, with multiple edges, etc. you would likely just be setting yourself up for a bigger fall later on down the track...

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Eobert,

 

Everyone has pretty much given some directions as to how and why the model you have is failing. Check out dimontegroup.com. They have some, though somewhat outdated by today's current functionality, it can still give you some major insight into what is going on behind the scenes in SW.

 

He gives a really good break down as to "why" the shell tool can fail. When you realize why it fails, you can then choose to not set yourself up to fail. (No pun intended).

 

You might also check out dezignstuff.com, he has a surfacing book that goes into all of the different features and explains WHY each one is what it is, and when each one works best.

 

As Paul said, it's not just SW that is the issue in that no matter what 3D program you use, Alias especially, there will be work "arounds". Anyone who tells you that they never have a problem in their 3D program also has a bridge to sell you in New York for $1.00. ;)

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Guest ChrisDuncan
Thank you for all the help and tips, people. I really appreciate it. Very insightful!

 

there's a nice tool in SW under "evaluate" it's called "check" it will find these "gap" disconnected edge problems and highlight them.

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