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Fillet Problem

Question asked by Dan Estes on Dec 31, 2007
Latest reply on Jan 14, 2008 by Brian Hoerner

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I am having difficulty filleting at the location indicated (surface prob.jpg). I attached a SolidWorks 2007 Part file for review.

I'm not sure what is wrong, because the surface indicated has been knitted (formed into a solid) and combined to the lower base. Is there something wrong with the sketches used for the surface profiles and guided curve?

Thanks in advance.

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Image.ZIP137.4 KB
Part4.ZIP775.2 KB

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Matt Lombard Jan 1, 2008 2:27 PM
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Do you have a particular solution in mind? Can you envision what you want the fillet to look like? Your part is not really conducive to a good fillet in this area. The partial dome is not exactly tangent to the base, which I'm guessing is causing a problem for the fillet feature.

Anyway, you can get a fillet to work by using a face fillet with a hold line, and using the outer edge of the flat face as the hold line. Again, I'm not sure what you have in mind for this, but it is one of a couple possible solutions. I'm going to guess that any other real solution is going to involve manually modeling in the fillet.
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Dan Estes @ Matt Lombard on Jan 1, 2008 3:22 PM
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I need a .50 radius fillet at the indicated location, but also along the edge of the face where the partial dome sits on.

You are probably right regarding the dome not exactly tangent to the base. I'll look into it. NOTE: The dome is supposed to be combined and sitting on the face of the solid beneath it.

Thanks.
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Dan Estes @ Dan Estes on Jan 2, 2008 3:50 PM
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I tried a few things (a lot) regarding the construction of the dome. - Still no luck. The dome construction on the attachement of my original post was was a surface loft. I have tried a feature (solid) loft, but no luck either. I need the dome to be aligned with the face beneath it.

NOTE: My sketch plane lies on the face beneath the dome. Should I create a new plane and re-locate the sketches below the face?

As Matt said, to get a good fillet or round, the dome should be tangent to the base, but I am still getting the same results after I corrected the error.

I'm open for suggestions regarding another strategy for constructing the dome.

Thanks again.
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Dan Estes @ Dan Estes on Jan 2, 2008 4:05 PM
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When I construct (surface, Knit and combine) the dome away from the edge of the face, the fillet and shell commands work great.

Again, what could I be doing wrong or should be doing different under the noted conditions?

Thanks.
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Ricky Jordan @ Dan Estes on Jan 3, 2008 4:30 AM
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Dan,

I'm not quite sure if this is what you are looking for, but I was able to get it to work by constructing a split line based on a curve starting 0.500" away from the vertex and then blending tangent to the curve at the end of the face. The split line curve is then used as a Hold Line on a Face Fillet. See the image below.

I have the file in SolidWorks 2008 format if you are interested.

Best Regards,
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- filletblend_1-3-08.jpg144.8 KB
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Dan Estes @ Ricky Jordan on Jan 3, 2008 11:29 AM
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Ricky,

The fillet on your image is what I'm looking for. Although, I'm not sure of the steps from your - "a split line based on a curve starting 0.500" away from the vertex and then blending tangent to the curve at the end of the face." I understand how to use the Split Line, but I'm not sure how to apply it to this condition. - Brain fart.

I am using version 2007, but thanks for the Ver. 2008 offer. Also, if I could see another image/s based upon your steps above would be greatly appreciated.

Hopefully the shell command will work once the fillets and rounds have been completed.

Thanks for your time,

Dan
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Ricky Jordan @ Dan Estes on Jan 3, 2008 1:05 PM
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Dan,

I'll try to put together a video showing how I did it.

Best Regards,
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Dan Estes @ Ricky Jordan on Jan 3, 2008 1:18 PM
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Thanks!!
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Matt Lombard @ Dan Estes on Jan 3, 2008 1:20 PM
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Dan,

The way I did it was to use the edge as a hold line, and you could do what Ricky has done with the split line, and use the split line as a hold line. The trick I think is to get the fillet to taper down to nothing at the point where the dome touches the other curved face. The problem is that SW can't extend either face - the dome or the curved face, so the fillet can't extend all the way, it has to taper to a zero radius sharp.

To use a hold line, you have to first create the split line, enclosing the blue face in Ricky's picture, then use the Face Fillet setting in a new fillet feature, select one face on either side of the edge you want to fillet in separate boxes, then go to the last panel in the fillet propmgr and select the edges of the split line.

It's a bit of a fudge, but its the only way your geometry can work. There is a convexity problem between the dome and that inset curved face.
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Dan Estes @ Matt Lombard on Jan 3, 2008 2:53 PM
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Matt,

"There is a convexity problem between the dome and that inset curved face."

I am doing a "reverse engineering" project. NOTE: Where the dome and curved face mate, it is noticeable between them. Are you saying there is a construction problem between the two. If so, please explain.

Thanks again.
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Ricky Jordan @ Matt Lombard on Jan 3, 2008 2:55 PM
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Using the existing edge as a hold line was the first thing I tried. It worked as well but it was taking over a minute and a half to generate the fillet. (Still not sure what was up with that.) The reason I created the split line was due to the desire to have the radius start out at 0.5". Using this method also resulted in a much quicker rebuild time for the fillet feature.

I noticed the convextity issue between the dome and the curve. I think another split line generated from a sketch onto the dome could fix that. It was getting late last night and I was running out of steam.

Another way to possibly do it would be to delete the faces created by the split line and then try to construct the fillet using a boundary surface. (Some additional surface trimming might be needed.)

I'm amazed sometimes how much work it takes just to get a fillet on a model.

Best Regards,
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Dan Estes @ Ricky Jordan on Jan 3, 2008 3:16 PM
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Ricky,

"I'm amazed sometimes how much work it takes just to get a fillet on a model."

You've got that right.

Dan
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Matt Lombard @ Dan Estes on Jan 3, 2008 3:32 PM
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See attached. The forum1 picture is your part. The Forum2 is mine. See the difference in the tangency? This is a deviation analysis. It looks like what is happening is that the edge around the base of the dome is first broken into many small edges, which is the first indicator of some approximation problem. Secondly, it looks like the edge goes from concave, then flips to convex, then back to concave again on the other side. This will always cause fillet problems.

My part doesn't do a regular edge fillet either, but it makes the hold line fillet without the long delay that Ricky is talking about, and doesn't break into a bunch of short edges.

The problem here isn't so much the software, its more that you're asking it to do something which is geometrically not possible with a regular fillet.
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- Fillet Problem.zip1.2 MB
- forum1.jpg29.3 KB
- forum2.jpg22.1 KB
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Ricky Jordan @ Matt Lombard on Jan 3, 2008 3:38 PM
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Matt,

Ahhhh....When you spoke of convexity I thought you were talking about where the fillet blends with the dome.

I did notice an awful lot of "short edges" along that edge where the dome was supposed to blend. I hadn't gone back into any of the existing features yet to see what was causing it.

Best Regards,
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Dan Estes @ Matt Lombard on Jan 3, 2008 3:52 PM
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Unfortunately, I am using Ver. 2007. I can't open your file.

Dan
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Matt Lombard @ Dan Estes on Jan 3, 2008 4:01 PM
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That's ok, you're not missing anything. It still doesn't do what you want it to do.

Either use the hold line fillet, or trim out a patch and make a Fill, Loft or Boundary surface to blend it in. If you want the fillet to continue around the tangent edge, it would have to flip convexity, and fillets can't do that. It can't extend either the top or bottom face because they are tangent or nearly so, and the wrong convexity to be extended if they could be extended. The only thing that is left is a variable radius fillet that you can specify manually with numbers or specify with a hold line.

This is why I asked if you could envision what sort of solution you wanted, because what you're asking for is not possible without a variable radius or a non-arc based blend.
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Dan Estes @ Ricky Jordan on Jan 3, 2008 4:16 PM
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When I delete the knited surfaces, the short edges were no longer there. Also, Is there a setting that is causing the concave/convex problem?

These are the steps I used to create the outer sketch of the first surface profile of the dome:

1. Created a plane
2. Created a new sketch
3. Selected the edge of the face
4. Selected "Convert Entities"
5. Constructed the remaining sketch for the first profile for surface loft

After the first surfiace profile, I repeated the same steps, but selected the first surface profile by selecting "Convert Entities". I then mirrored the new sketch to the other side of the dome. After that I constructed the sketch for the height of the dome. Then I created the guided curve on the back face of the dome.

Is there a problem with the initial construction?

I'm becoming more confused the more I get into this.

Again, thanks for your patients,

Dan
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Matt Lombard @ Dan Estes on Jan 3, 2008 4:46 PM
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Dan Estes wrote:

When I delete the knited surfaces, the short edges were no longer there. Also, Is there a setting that is causing the concave/convex problem?

Yes, deleting the knit would remove the short edges because it blows up the Combine, and so you are talking about different bodies. There is no setting for the Concave/convex. It is a problem of technique, which is why it is so hard to describe a "fix". You have to approach the problem differently.

These are the steps I used to create the outer sketch of the first surface profile of the dome:

1. Created a plane

2. Created a new sketch

3. Selected the edge of the face

4. Selected "Convert Entities"

5. Constructed the remaining sketch for the first profile for surface loft

I'm not trying to accuse you of anything, but you've left out some steps. The spline that is there is a proportional spline, and it doesn't have any On Edge relationship. You've defined it with dimensions. The spline's relationship to the edge is missing, which is probably what is causing the short edges. In the part I built, I built directly from edges, without using converted splines. This makes the intersections cleaner.

The 0.050 gap is the one that really gets me. You can't really get away with this if you want perfect models with swoopy shapes.

After the first surfiace profile, I repeated the same steps, but selected the first surface profile by selecting "Convert Entities". I then mirrored the new sketch to the other side of the dome. After that I constructed the sketch for the height of the dome. Then I created the guided curve on the back face of the dome.

Is there a problem with the initial construction?

I'm becoming more confused the more I get into this.

Yeah, you're confused now, but eventually you'll learn something from this. Surface modeling is not something you can just fake visually in SolidWorks. Stuff has to be mathematically accurate, perfect even.

Again, thanks for your patients,

Dan
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1-9C36HC Jan 3, 2008 4:52 PM
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Dan,

This caught my interest because I'm working with documentation to get a submission into online help about how to use loft vs. fill and "Singularities" that result from doing 3 sided lofts and boundary features.
Your example can be accomplishe with a variable radius, but... the method in which the nose area is created needs to be changed. I would argue that you shouldn't use a loft to do the upper shape because it creates "singularity" or a degenerate point where the three loft profile meet (you can see this if you edit the loft feature and have mesh turned on) and would cause downstream problems such as shell and filleting (even thou we sometimes overcome it with our shell feature.)

See attached file.

I just realize that this is 2008 SP2 in which you don't have yet. So download it and save it for when you have it. In any case, these are the steps:

1)Forshorten your Cut-Extrude1 to 30.31 from origin so that you don't cut away the tip of the nose area. (also consider redoing this upper shape as a fill feature or cut away the end and patch it with a fill.)
2) Using sketch32 Create 3 transistion curves between it and the vertical face of the cut.
3 Create a boundary surface using the cut face, Sketch32 as the 1st direction, and the three curves you created as the second direction.
4) Create a planar face from sketch32, copy-offset by 0 the vertical cut face and create a 3rd planar face from the open profile of the two and the boundary surf.
5) take these 3 surfaces and knit solid to the boundary.
6) Combine it to the existing solid.
7) Now you can apply Variable Radii with a start of .5 and end of 0 on either side.

One of the other problems that occurs with your current method is the "dirty edge" that was created as a result of the loft and then subsequent Combine. You can use heal edges Insert>Face>Heal Edges to clean this up but was "too dirty" to make it a single edge. This is a ParaSolid/SolidWorks issue with model tolerance that we are working to overcome. In the meantime, Boundary is more accurate than Loft, that's why I used it.

Anyway, I apologize for the unreadable SW version here. SP2EV is out if you want to download it and then read it.
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- untitled11.JPG75.5 KB
- Fillet Problem-mab.zip883.7 KB
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Brian Hoerner Jan 3, 2008 5:43 PM
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The real answer to this is the clay-dremel-sand command (I have been asking that all the way back to IDEAS-1)

Imagine that, selecting a tool that could just rub that edge the right way, of course the virtual gloves have to come on first

Not trying to make too lite of a serious discussion, just some jocularity for 2008....hope it is great for all!!
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Dan Estes @ 1-9C36HC on Jan 4, 2008 11:25 AM
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Mark,

I am having difficulty trying to locate SP2EV at SolidWorks's website. I did a search, but that didn't seem to help. Am I supposed to contact my re-seller?

Thanks.

Dan
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Matt Lombard @ Dan Estes on Jan 4, 2008 12:57 PM
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You're not on the early visibility list. You can sign up for it here

https://www.solidworks.com/pages/services/subscription/EarlyVis.html
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Leonardo Sanchez Jan 4, 2008 4:05 PM
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Can't help but wonder if you might have had a smooth transition on your mind
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Dan Estes @ Leonardo Sanchez on Jan 4, 2008 7:29 PM
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Looks good!
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1-DNQF8W @ Dan Estes on Jan 7, 2008 3:14 PM
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Hi Dan,

It´s not the cleanest solution, but without any further surface tweaking to your model I could generate the result shown below. Just add a Variable fillet and give a value of 0.5/99.99% the control point next to V2 (Try 0.5/100% to see if it suits you best). Just remember to add the value of 0.5 to all the 4 unassigned points exept the last one (V2) wich should be 0in.

Hope it helps.

Regards,

Ricardo Kossatz.
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- varfp.JPG9.8 KB
- varf.JPG38.4 KB
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