Merge Smooth Faces Problem

I'm looking for any suggestions or tricks that will allow me to enable "Merge Smooth Faces" in a sweep in which the profile isn't directly pierced to the guide curve.

Here is a simplified example...

If I change the sketch segment (as noted in the file) from a solid line to construction geometry (which is what I would like to do), the Merge Smooth Faces setting enables itself for some reason, causing my sweep to change and even fail in some cases. Worse yet, it's grayed out. Why is this?!

I need this setting to be disabled for a particular project so that the sweep follows the guide curve precisely. When it's enabled, the sweep is very sloppy as can be seen in this example when you modify it. When you edit the definition of the sweep and exit, it gets even worse.

I hope I explained it well.

Any help would be appreciated. Thanks! Mike Wilson

Yes, I do need the full circle, unfortunately the profile is swept along a 3D spline. I would have to possibly do a mirror part and insert it.

I even tried sweeping two concentric circles and still the same problem. Wierd.

Thanks Arlin for the feedback!

Mike

Mike,

Yeah, wierd!

This is something I never have liked with sweeps. There is no control for the normal path direction within the sweep feature, you have to build/construct it. So, in this case, the vertical solid line is controlling the normal and it seems to loose it when it turns into a constuction line and if you build a normal plane for direction, it forces a smooth which is grayed out? Sweep needs a overhaul. It should have some controls for the start and end conditions.

And as you probably have noted, it fails in SW2004?

Flaky for sure.

Mike the problem comes from the way the surface is constructed-if you make with a solid line you will notice if you scan through that the sections they become constrained to the proper points to define both surfaces- however if your line is a construction line then the sections become spaced along the path and do not land on the points you intend for which sw then tries its best to form a whole surface from. the fix for this is to change sketch 1 by selecting your arcs and making a copy offset 1 inch in y direction, change the original arcs to construction and then head to sketch 3 to redo your pierce point to intersect the new guide and the outer profile-hope that makes sense cheers

I definitely see what you are saying, unfortunately, my arcs are going to be a 3D sketch so I can't do a copy offset. Your idea has me thinking though. I may be able to do the opposite and offset my path instead. Let me try that and see what happens. Thanks!

Mike

Paul, maybe I'm reading you wrong, but this is a new feature of 2004; you can assign a direction for the sweep using a vector- etc. Thank Jim Wilkinson and others who sneaked this in a few months ago after I did a presentation in concord showing how Pro uses "pivot direction" in Variable section sweep to accomplish this. This feature is working now, although it wasn't in Alpha and Beta1. It should allow you to sweep profiles with only one path without it twisting abnormally. It will be invaluable for building draft surfaces for loft and fill etc. To the other problem with "merge smooth faces", it is a bug that I've submitted and although I haven't yet loaded SP0 sounds like it still exists. The problem is that when you sweep a profile with a path, w/o a guide curve, you don't get the option to smooth or unsmooth. The check box is checked to smooth yet the faces don't merge. If the checkbox shows it smoothing it should smooth even though its an option under guide curves.

BTW, heard that you've done some work with Studio Red down here. I might be training some of there people next month.

The other new feature in 2004 that hasn't been talked up much is "Ruled Surface" I've been using it a lot. It also a great "construction" surface feature and saves a lot of time of creating sketches (can create surfaces w/0 any sketches or curves). If you haven't tried it check it out.

Hmm, you can do it in SW2003 as well using a plane, vector does not seem to work with either SW2003 or SW2004. Or am I missing what is different aside from the example here?

Well, I'm glad they are sneaking some stuff in. (wish they could sneak in some more insert part (data sharing) capability/management) Would you have a simple example?

Hmm.

Yep, they're one of my clients. Some very good people there. Just as with ideo and the other design houses, they're getting more SW work.

I just started to explore SW2004 and I very much appreciate some of the new stuff that has been added!!

later..

I understood you could copy/paste 3d sketches...and then just translate/move it? but it will be a new sketch to 'stitch up' under the sweep. I don't know what you are working on but you need to translate in y direction rather than offset?-which I realise cant be done without making intermediary offset surfaces and converted entities

I see! I figured it was a limitation.

I experimented a little with this, and I will definitely put it to use.

Cheers, Mike Wilson

I recreated Mike's model with some methods that are a little more robust (I think).

I believe part of the problem with Mike's model is in his 3D sketch paths, he uses curve through surface intersection. The way his surfaces are modeled, this can create 2 curves in the path. I assume Mike deleted the extra entities when creating the sketch so there would only be one curve path. However, when the model is changed and/or rebuilt, the extra curve can show up in the 3d sketch again, failing the model.

?!!NOTE!!? I also created this part in SWX2004 SP0.0. It worked exactly the same as 2003, I never even crashed once in a couple hours of toying with these models and modifying them!!! BUT.... The model created in 2004 is ~50MB and the 2003 model is

Oh yes, I forgot to add you must unhide the last surface body.

When you sweep a profile along a non-linear curve like a 3d Sketch, you now have the option for the profile and all of its constraints in the sketch to sweep "relative" to a external reference that you select. Take a look at the following part:

ftp://public.ideo.com/blind/sweep-w-path-alignment.SLDPRT

This file will be removed in 72 hours.

Hey, I think I got it. This is pretty much what I was trying to accomplish...

I found a way to incorporate your translation idea, but in a different way.

Thanks again! Mike

Hmm, it fails with a ctrl-q using sp3.1 And it fails in SW2004 but in a much different way. (hmm, "path alignment type" seems to be dependent on the type of sketch setup?)

BTW, isn't this a similar flex hose the ng was doing (end of mar 2003)?? And similarly, with the ones I worked on it would fail with a ctrl-q, I just looked back at some of the ones I did.

..

no problem here with rebuild sw2003sp4

yup I have 9 parts now in my download examples

well that's odd...I checked again twice and it works here....hmm...

Yes, this is what is happening. Nice development, Arlin. It has a few more steps, it's pretty clean and I'm able to twist it without failure, it is very stable!!

Interesting, in May, I think it was more/less about trying to minimize the feature list and after looking back some of the models, it really comes done to more features to increase stability for this geometry. That is, looking back, "merge smooth faces" is what this exercise is all about? Getting around a sweep limitation?? Man, we bang our heads on something way too long. Sweep is limited, period.

Yep, it's true!! I've been watching my old models growing and growing and growing... It's insane! Hey SW Corp, what is the deal??

Also, I'm curious, what happens when computing goes to 64 bit or is SW2004 showing the first signs of this???

..

I like it! For some reason though, if I do a CTRL-Q in 2004, the profile sketch shows a warning.

I just made a quick guess that maybe it has something to do with materials or textures in 2004. How much of that info gets stored in the files?

I did a sample part and the size did go up after applying a texture, but I haven't really experimented too much.

Hopefully a new version of EcoSqueeze can help solve this problem, even though SolidWorks warns us not to use it. .

Mike Wilson

Yeah it was fun to see how it could be made in the fewest features.

Originally, I didn't even realize that the merge smooth faces toggle would help, since no one mentioned it. Then the other day I was playing around with that feature and figured it could help out with the hoses by making the sweep a little more crisp and defined.

I never used the term "workaround" until I started using SolidWorks ;^)