Hello,
I am working on an exhaust manifold and i am facing some difficulties creating boundary feature. As you can see from the picture, I am cutting the runners and the turbo flange and want to connect them using boundary feature, so the model has better shape. No matter how deep I cut the runners, every time I get the strange creation circled in red on the second picture. Can someone help me with this and explain why this is happening and how to fix it, please?
..yeah unfortunately, after a ctrl-q.. this model fails and when I try to edit or add to it, it keeps giving me errors... so, there is more to do to clean up (turn VOR "on") (I don't think the under defined sketches have anything to do with the failure)... also, imho..I don't see a reason to blend tangent with the end mount.. just have tangent to the tubes and blend (add radius or another blend) at that rectangle later?
I didn't open the file, it seems the comments here already have things covered or sorted out, just need to put in the labor to accomplish it. I would like to add into Paul's comment about VOR, Verification On Rebuild.
The latest example or problem I experienced with this is I opened another user's file, I created a new sketch on a flat surface, converted entities to temporarily have some reference dimensions to have an accurate or good starting point for a mating part's sizing (it was an irregular shape, like an angled ellipse not easy to dimension), and upon doing this, or editing the file in any form, there were features that would break and not resolve. It was tracked down to one sketch contour or entity(ies) in one feature that was to blame. This sketch was copied from another part and added into this part. So it's initial copy could have been bad, or the paste into new part bad, just some not ideal behavior on top of another not ideal behavior.
It is better to have VOR turned on or the box checked like the attached image. I run into this problem too often when working with other members, it's not a problem for them when this is turned off, but it's a problem for users that have this setting on. The simple, easy, lazy, and wrong and not thorough solution is to have VOR turned off, but this caused problems downstream and also is a subpar quality item. With it turned off the software only checks locally on the immediate feature or changes being made, so there may be a slight performance improvement but at a cost. With VOR turned on the whole model is checked globally, not just locally, for errors.
VOR off = maybe good enough, problems will come later for myself or someone else, hack it together
VOR on = Proper way to go about things, handle any problems that you can capture on the front side of things so can cruise later on.
Jesse Robbers well said!
I really wish ALL Users and Managers were taught and reminded often, "with real world examples", about VOR,... it seems SW Corp hides away from VOR (we don't want to go there)... and the VAR's have to deal with it.. writing in blogs on what it is about?
Also, the Users need some VOR Icon Warning option stating the files used were not created with VOR On.. (or vice versa, Off?)
"Do you want to Rebuild with VOR On?"
My opinion is to remove the option of VOR on/off, make it on by default. If you're doing the design/engineering type of work, you should be up front or able enough to do it the right way from the start. With it turned off, it's like having beer goggles on, getting something made on a Friday or Monday, guess it's OK, send it thru. It being turned off causes problems and you have to first inform individual(s), then show the problem, then teach or instruct what VOR is, then instruct how to fix the problems that were permitted to be created, then instruct how to avoid problems in the software due to better practices.
If having this off really has any value, it should not be a hidden setting that causes problems due to practices between users sharing data. A 'draft mode" option or setting with things dumbed down may be a better approach. One that kind of groups VOR on to be off, zero thickness issues, draft, min curvature/shell issues, all of those type of things grouped to be toggled off or a no warning just to be able to hash out some quick proof of concepts. Then to design further beyond this stage, the file goes from a draft mode type file (kind of think educational vs. normal license) you evaluate the file (the software does this) with VOR and these issues on, or start from scratch looking at the near end solution and do it from the start the proper way so it's stable and efficient in the long run for possible future released rev's.
Hello Jesse,
All excellent points! Taking VOR away... has been discussed over the years.. but seems to go no where but I do see options if they (SW Corp) does not...
For the EDU license, call me a nazi but I would enforce VOR ON. (sorry Georgi, I get tired of seeing issues)
From a single user professional point of view, I have my reasons at times to either play or be serious with the data, I don't mind the choice but I want to be Warned There Is a Conflict with the VOR On/Off setting, especially when I open/work on other peoples data.
And, from a corporate perspective/control,.. a option to LOCK VOR On within the license group,... maybe a smart management option?
I too have issue with this option turning on/off in many of my surfacing model
The model might have some weird shapes when it's on and back to normal when it' off
Will this be accepted?
Apply split lines on the surface to isolate the area and then use the delete face command with tangent fill option.
Newell Voss wrote:
Apply split lines on the surface to isolate the area and then use the delete face command with tangent fill option.
Excellent - It's quick fix
Hello and thank you to all who answered.
Alex Burnett: I was thinking also for guide curves, because I want to have more control over the shape.
Paul Salvador: I am not sure why it fails on your end. I don't have problems force rebuilding the model.
Christian Chu: It is acceptable, but I still don't like the transition, also there are few more areas that I want to correct.
Newell Voss, Christian Chu: This is what I did first, and yes it as a quick fix, but not the right fix for me.
The interesting thing is that the problematic area shows when I start adding connectors. I am adding them in order to try and control the curvature, but at some point when I and one this thing shows up and I can't get rid if it.
Now I want also to cut more on the side of the runner, so I can make the transition better and this time I will use guide curves. I will let you know when I am done.
Thank you again to all.
As Alex mentioned in his post, you need to create some guide curves to have a better curvature
What I've done with you model was to adjust (reduce) the tangent length to provide more space for the surface to blend
From the model, I guess its a (metal?) casting part - why you need it super smooth (C2?)
I took a look at the file and my main suggestion is that you're going to need some guide curves. Any time that you try to create a boundary boss of one profile to another, solidworks will almost always do it "wrong". Create a 3D sketch of splines that connect the first profile to the 2nd profile. This will help you control tangency as well for some of the surfaces.
Side note: The majority of your sketches aren't fully defined which makes it difficult to work with. It's best to fully define everything, every time.