Swept Feature 3

[lurks]

I am trying to sweep this feature down to a point while staying tangent to the outside edge of the part. I have attached a picture of what I am working with. Hopefully someone will understand what I am trying to do here. Any help would be greatly appreciated. Thanks in advance.

Lurks

 

[lurks]

Okay, I got that straightened out but now when I am trying to sweep it as a solid I am getting an error message that says the Reference Coordinate System is undefined. Does this make any sense and how do I define it?

 

[hudson888]

Lurks,

I've been meaning to reply for a while but I had something on and wanted to take the time to set you up with a decent attempt. Also I knew this was a bum task before I started so read on.

You know how sometimes no is also an answer. Well this is one of those times. What you're trying to do is to create geometry that disappears to a point. This is something that NX abhors with some justification. So even though it seems simple when you say that I JUST want to do this, I'm afraid that you've stumbled upon a case which is a near impossibility and even when we do make it work it isn't very good.

John knows this well enough I'm sure and he tried to steer you to a couple of examples that involved more straightforward and better resolved methods of constructing the geometry in question. In effect he says you probably don't want this instead you would be better of with a more sensible alternative. I agree with him but I give you a result that approaches what you asked for nonetheless. Keep reading to find out why I don't even like my own model.

Michael gave you a swept feature as you asked and he did a pretty good job of answering your question with that. So I don't want to bring him down with anything I'm about to say because it isn't his fault that NX just can't do a good job using this technique and especially not his fault that he used your bridge curve which of itself introduces some problems.

That bridge curve in shape if you look really carefully in plan view goes outboard of the existing profile. I guess you didn't know that at the time and it is pretty much going to cause huge problems controlling the shape of the outboard portion of your sweep. I used it in part but later added an extra curve in the center of the tapering section to better control the blends.

The other problem with the sweep is that it goes down to zero and this as I mentioned gives you no control over the faces as they approach the pointy end. You have poor tangency between all the faces edge to edge and back to the existing face at the start. In fact the outboard side of the swept feature which could be assumed ought to match the side of the base does not. Instead with bellies out by 0.018".

The problem with wanting to come to a point is that a three sided surface is anathema to NX (in common with most if not all other CAD systems). Surfaces like curves are controlled by a their vertices or poles as they are often called. When a rectangular surface is built poles in the U and V direction are matched end to end and side to side to create a mesh. When one side consists of a point therefore you have the situation where all the poles on the opposing side have to meet just one control. So as the resulting surface nears that point somewhere within the tolerances that NX builds to there will be some lack of control. In fact you almost never get a desirable result.

I've tried to repeat the same sweep that Michael created with equivalent effects using an improved set of curves. This was after I created what I'm sending you now. The result was a little better but equally could not be united to the main body. We both had that in common, and the reason as I outlined before should no longer surprise you, of course the face at the bottom, (the underside as you look at the model), would not match the original. We weren't able to assert sufficient control over the swept body to ensure that would be the case.

What I have done is to sweep an extended version of the top face using you bridge curve, just to respect the geometry you intended to create. I closed the shape with some extruded sides and extracted faces. These I may have removed parameters from for convenience sake as it was only a quick method. You should probably alter your sketches etc.. to a better job, but I think you're better able to see the method behind it if I just explain that this wasn't very important and leave it so. The result was a sewn body that has five sides tapering to a point and having sharp edges. I also mirrored it before uniting this to the main body to do both sides. The other thing I haven't mentioned thus far is that I removed some of you original blends and united my new solids to your main body at an opportune point for me to reattach those blends before another feature. This was done because my means to create pointed ended blends was to use tangency controlled face blends. The new curve I talked about earlier was just a curve down the center of the tapered solid in plan view that I projected in Z onto the face. This I combined with edges that I took off a temporarily applied edge blend (0.125" radius) were the tangency controls for the face blend. And on the outside another tangency controlled face blend also came to a point and there you have it.

I reapplied another blend that needed to go after and I deleted a couple of faces (simplified in NX-4) that aren't required and it appears to be an Okay result.

However checking some of the blend tangency it still isn't 100% perfect. I'm seeing isolated errors near the pointy end of between 3 to 5 degrees 'ish. Normally I wouldn't be happy with that but to prove the point without dodging the fact that there are limits to everything I would say it may be just about the best you're going to be able to achieve.

I hope you get something from this it was an interesting journey. Next time I'll send the you a bill

Best Regards

Hudson

 

[mmauldin]

Hudson,

Your explanation does not bring me down at all. In fact I agree with your explanation 100% and applaud you for taking the time to explain it in detail.

My submissions were more to show a method of creating the desired surface rather than a commentary on it's appropriateness, and as I said I took some liberties creating one of the guide curves (a simple 5 or 6 node spline) with no assumption that it would match the side wall perfectly. I was able to join the solids by offsetting the "mating" faces but as you would expect, the results were less they optimum.

As a general rule, personally I would seek to create a geometry entirely from primitives, feature, blends, etc. even if that required tweaking the design and resort to the use of surfaces when all else fails. For the most part this approach results in a more stable model.

 

[hudson888]

Thanks Michael,

I'm glad that you see it that way and I have to agree that the better overall approach was along the lines of some of the things that John tried to point out. I would be more comfortable either going close to being at a point or close to being tangential to the other edges at the base but with a slight angle and a small radius the appearance might be similar and the break in tangency could be smaller that errors that we currently have anyway with my best attempt but with the rest of the model more properly controlled. I'll see if I can model something later and post it up for discussion.

Best Regards

Hudson

 

[lurks]

Hudson,

I appreciate the time and effort that you put into your response, it proved to be very helpful and informative. Through observation of your model I completely understand the logic and method behind it however the part that I am lost on is when you created the sheet bodies that show up on the model tree as just "body". How was this done? Where is the tool within UG NX4 to perform this? Thank you again for all of your help.

Joe

 

[hudson888]

Lurks,

A couple of things about it that you wanted to know. I kept the parameters for the swept feature because I knew you would want to verify what I did. The sweep in itself was not particularly interesting or well controlled. It matters that it is tangential to the top face of the wall or rib feature but as it comes down to the base at a point the orientation at that end is scarcely relevant in this case. The sides were simply extruded vertically or up Z if you like. The outboard side comes from the edge of the part, and there was a wound line after I united the sew result so I simplified it away. The inside face was one of your bridge curves. The rear and bottom were taken from extracted faces, you can see that I have trimmed some of the sheets and kept the trims, then sewn the five faces together to make a solid. It was just that I realized that I really needed to insert these features into the middle of the model a bit too late and decided to take a few short cuts that I blew away some of the parameters simply because there were one too many dependencies for convenience sake. I'm hopeful you'll follow the explanation as the early geometry was fairly simple and I just wanted to point out the use of face-face blends as a more reliable technique.

I have had quite a bit of fun with you part and even tried it in other CAD systems with some success. There are always arguments raging about whose system can do what that we like to explore whenever we're not totally happy with the results were getting from NX or vice versa.

In this case I would simply comment that a three face to face blend might have come in handy. The deficiency however is slight because the need of this kind of geometry crops up relatively rarely.

I'm not sure what your part function is or whether I'm correct in guessing that it is a molded part that may as yet lack draft. In that case you'll have to reconstruct some of the geometry before you're done. If you want to continue with this thread we'd be happy to explore those solutions and alternatives should you feel the need. I have looked a little further and suspect you may eventually do better to resolve that corner that tapers but does not need to come to a dead sharp point, in which case we can get resolved blends to run right around including some of the other edges that we had currently left sharp.

Best regards

Hudson

 

[lurks]

Hudson,

I would definitely like to work on alternate solutions to this particular part in the future, but for right now I need to just finish what I am working on. You are right about this being a molded part in fact it is a cast ductile iron piece. It is implied on a cast part that there is going to be 3 degrees of draft when it is produced. I do have one final question for you regarding this part though. I have been playing with this even further and have everything exactly the way that I want it and am now having trouble applying the face blends to the rib feature. I have tried many different methods of doing this with no success. Is there something in this model that makes it impossible to do, or am I just not doing something correctly? Any help would be greatly appreciated.

Thanks again,

Joe

 

[JohnRBaker]

What size blend and could you show us exactly where on the model would the blend go?

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[lurks]

The blend is not going to be a constant radius but tangent to the centerline of the rib at the front of the part. What I mean by this is from where the three faces converge at that point if a line was drawn that at any given point it would be at the center of the two faces. Does that make sense? Hudson had created it on a model that I had posted earlier in this thread, but I was unable to duplicate it on this current model. I have attached the model that Hudson was working on that he had used a face/face blend to create what I am looking for. I have tried to create curves that would act as a tangent curve for this type of blend with no success. Thank you again for all of your help.

Joe

 

[JohnRBaker]

Do you mean like this...

But be warned, you have some poor geometry in some other parts of your model that is going to cause problems much larger than this one. I suggest that you run Examine Geometry and test for 'Tiny' objects.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

Lurks,

The geometry problems that you want to be aware of will include tiny objects, but according to the standards that we work to spikes and cuts are never permissible. That was part of the reason why I elected to go with the face-face blends, because the ordinary blends being non-tangent controlled will meet in the top middle where you have regular geometry but elsewhere they alternate between overlapping or leaving little slivers of top surface that you probably don't want.

Now where will the shut face be? on the very bottom face or at the base of the wall you're blending.

Next is it your intent to keep the 0.125" radius on the top of the rib, or would you be just as happy to taper up from the base of the rib just so long as the radius winds up half and half?

If you try to keep the radius that I build you would take an isocline curve at 3 degrees and experiment with either an extrude in Z then taper or a law extension at 0 or 180 degrees from the blend surface. Then you'll find that the tip being less than perfect, (which I told you it was), will eventually lead you to rebuild the sides and re-apply the face-face blend in order to get back to something like acceptable geometry. I would use the top say half of the isocline curves and then rebuild the end that comes to a point with bridge curves or studio splines as construction geometry for new sides.

More importantly with the above you will find the applying taper or draft from the top of near the top of the rib will result in faces which flare out to the base of wherever your shut line is. As the rib ends the taper will reduce to the point, but since other parts of the base have no taper may be tapered from different heights the profile of the base needs either to change to reflect that or will wander and step in and out wherever it comes to a shoulder.

That's why most people set the shut-line in place to start with and blend at the end of the process.

I was going to attach some images for you to work with but the server is balking at that , so think about this lot and I'll try to find some time to experiment more with this model over the weekend.

Best Regards

Hudson

 

[lurks]

Hudson,

I am trying to use the same tools that we have been working with on a different part. I have three guide curves and two section strings but I am getting some interesting looking curves to say the least. I have tried this a number of ways and I think that I am using the correct method but then again there could be a method that would be better. Thank you so much for all of your help, I know that I have been a pain.

Lurks

 

[hudson888]

Lurks,

These are images that I was talking about the other day. Now you have sent through the drawing I'm starting to see what you're dealing with and why you're having some trouble with it. It looks to me like you're dealing with older drawings of cast items and that they have been drawn without draft. Some of the dimensions probably don't even work properly when you attempt to model them in CAD. They will be even more difficult when you attempt to add draft.

View the images with the text of my previous post, and have a good think about the question of draft. If you want apply it then I'm urging that you do so before the blends. If in the past it was added by the molder or toolmaker then you can bet that the blends were likely to become subject to change rather then the profile of the shut line.

Some molders don't want you to apply draft, and if they're working off a dimensioned drawing then you'll understand why. Problems do occur when they decide to nominate a split line and draft the thing contrary to what you want to use as a datum to setup your machining. I prefer to draft my models, and that way I get to nominate the split line.

At this size they're more likely die-cast than sand molded anyway so an NC machined tool is a reasonable proposition. In fact I could guess at investment casting but thats really your concern not mine.

I'll attach something else for you on the other model as there is already one attachment to this post. You need to address the draft question before we try again on the first model.

Best regards

Hudson

 

[hudson888]

Lurks,

Now with this one I have more or less done what your previous work suggested. Boy that drawing is hard to read. I don't think it shows quite what you modeled. So perhaps you're making and improvement on the original design.

As regards the sweep I could have swept the whole profile in one feature and initially intended to do so. However I found that the extrude then the sweep provided a better controlled result that I was happier with. I have added something according to the drawing which looks relatively similar on the other end of the same groove. The construction is on layer 21.

On Layer 22. I took an extracted body at timestamp (exemplifying something I think you mentioned in another post). Then I tried to use a face blend to a side view profile more or less according to the drawing. NX will mess up the tangency of the faces within these blends if you're not either careful of lucky. In this case we had a dearth of luck and I'm not recommending that result for you to use for that reason. Sometimes our failed examples are the most useful so I left that in the file on purpose.

If you do want draft on the model then take the rads off the sketch, nominate a split line and start again. Apart from anything else you can always apply blends after you extrude so I prefer to have the option to add them later on some occasions. If the radii cross the split line the opposite may be true, but you still get that opportunity if you extrude blend then taper in some places and blend after the taper in others.

I noticed that you're going to have trouble with the outlying grooves on either side. They don't seem to fit and this is partly because the sketched extrusion that they're subtracted from is narrower that the drawn dimension. I still wonder whether you will get the blend to fit when it is corrected. Sometimes you just have to work to the "Spirit" of these older drawings.

One last small point of etiquette when modeling for others to follow your method. Don't boolean with your feature creations (i.e. extrude with subtract), it is not as easy to work with. Some will disagree with me I know, but it is generally a safe assumption.

Good Luck with your project.

Hudson