hidden lines (drafting) in NX5

[Crocostimpy]

I've searched around and couldn't find anything else pertaining to my question. I want to 'erase' some hidden lines in a drawing view but can't because the edge continues around the part and becomes a solid line that I don't want erased. Picture the threads on a beverage bottle. I want to get rid of the line(s) on the back of the thread, but because the sweep that created them winds around the top of the bottle (sometimes multiple times) that line is considered one whole entity.

Is there some way around this? I need to have hidden lines on in the view because there are other lines that I need to show. I've been searching around trying to find some way of 'splitting' the lines so I can erase the ones in back, but haven't had any luck. I've been using View Dependent Edit to Edit Objects.

Any help (or sympathy) appreciated. ; )

Mike

 

[ewh]

View Dependent Edit -> Edit Object Segments

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[Crocostimpy]

Boy, the one thing I didn't try (because I thought I had to have the lines divided into segments already)!

Maybe I'm doing it wrong, but my problem with that is I can only select one line at a time. I pick Edit Object Segments, then change the line style to be Invisible, and then Apply. I can select one line, and when I try to select another I get a Point Is Not An Object error. I get the same error when trying to select any other line. So I could keep doing that over and over again I guess one line at a time.

I did just find that I can divide the faces in Modeling, and then when I go back into Drafting I can select all of the hidden lines I want to erase all at once.

Mike

 

[ewh]

You have to approach it one segment at a time. Pick the curve, then pick the boundary(s). The cue line will tell you what is expected next.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[Crocostimpy]

Ok thanks. I think I may like the divide face option better. It's certainly quicker if you have a lot of segments to get rid of.

Mike

 

[ewh]

View display is much more robust than it used to be, so I don't complain too much. ;-)

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[hudson888]

Crocostimpy,

On reading through and spotting ewh's post the point is well taken. In fact should you be having too many entities that you need to view dependently edit in this fashion, then you're probably doing something wrong with the hidden line removal settings. If you think that may be the case by all means ask or even attach an image it may be that something as simple as toggling a switch or change a tolerance here and there could save you a certain amount of extra grunt work.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Crocostimpy]

I have played around with the settings with no luck, at least for my needs. I'm attaching an image of what we call the finish, or the threaded part at the top of a bottle. You can see that because it has numerous turns and because it's an interrupted thread I'm left with lots of little hidden lines that I want to remove. Because the dashed lines in the back come around the bottle to the front, they will disappear also when I erase the dashed lines. I can use the Object Segments option, but I have to do each one separately, which will be time consuming.

Trying out the various hidden line settings either all of the hidden lines in the view disappear or all of them stay. Remember that there are some hidden lines that I want to keep, so I can't just turn them off for the entire view.

So far dividing the faces seems to be the quickest way to do this. At least as far as I have found so far.

Mike

 

[ufsure]

This is a workaround. I would set this main view boundary to be manual and clip it just below the threads. Add another view with no hidden lines and make its boundary such that the threads are visible and just overlaps the main view. The views can be easily aligned by using the overlay method. You will not have any problems dimensioning, but if you section these views you may have to adjust the view boundary of the section view.

Suresh

http://www.technisites.com.au

 

[ewh]

While not intuitive, Suresh's sugestion may be more efficient.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[hudson888]

After seeing the image I think I'd also do as Suresh suggested it just seems so much easier than fighting against what the system wants to do. To split the views try placing a line to use for a break line detailed boundary.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Crocostimpy]

That sounds like a good solution, but I'm not sure I want to leave a drawing like that to confuse the next unsuspecting designer to make changes to or use as a starting point for something else. Particularly if I'm not around in the future to explain what I did. Since the overwhelming majority of our finishes are standard imported parts, once I divide the faces and save them out again they'll always show up ready to go after that.

Mike

 

[hudson888]

Mind you mike based on your image there is no other visible area where you seems to actually want to have dashed hidden lines. If you just want to show the broken thread in more detail then perhaps using a lateral solution turn the hidden line display to invisible and cast the odd extra partial view to clarify that detail or even a detail view in a circle with the hidden line set to dashed might be convenient for you.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Crocostimpy]

That was just a small piece of an overall view to show the area I was talking about. We always want to show what we call the pushup, or indent in the bottom of a bottle, in the views on the drawing in hidden lines.

Sometimes they're simple like a dome, in which case I have just used an intersection curve and changed it to dashed lines and then showed that layer in the view, keeping hidden lines off for the whole view. And sometimes the pushup is complicated, like a water bottle where it may have numerous flutes. Those are the cases where I need to have hidden lines on for the view, but also need to erase all the other hidden lines.

In the previous CAD software that I used I could turn on hidden lines for the whole view, then select the lines I wanted to keep as hidden, then turn the rest back off. That was real easy. When I started using NX I had hoped that I could do somewhat the same thing, but I can't. Oh well.

Mike

 

[hudson888]

Remember what I said earlier in that you can do some of it with standard detail views and sections.

What you're asking to do is something that you could I suppose request as an enhancement, because it sounds pretty cool. Before you do that you probably need to understand is that it simply isn't standard drafting practice to support such a method, so your request may be politely declined. In fact I probably wouldn't support it myself.

If I'm right then anyone reading the drawing as you have shown it in your attached image might be entitled to presume that the bottle was solid and not a hollow shell. Even if I'm off in this case then you could possibly imagine other circumstances where the design could be misrepresented for convenience sake in ways that are simply incorrect. From a draftsman's point of view you may be confident that you know what you're doing, but from a drafting supervisor's standpoint I'd prefer to adhere to standards and know that my people were going to stick to representing the design in the most reliable fashion. That's why I'd rather see the detail views or section used, because the intention is clearer.

I don't mean to say that drafting standards should not perhaps adapt to what the technology is capable of supporting, but it is important not to overlook the potential to discard clarity in doing so. Some would disagree and insist that the draftsman be qualified to decide how and when to use the tools. I tend to think that if there is an equal but clearer method then the better judgement was to use that anyway.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Crocostimpy]

Well, all of our models are solid. There's no real reason for us to make them hollow, particularly at the thicknesses that we would need. I'm pretty sure it's the same industry-wide. Besides, I haven't seen a CAD system yet that can offset a completed design without fail. All those radii and small surfaces tend to screw them up.

The layout of our drawings was established long before I arrived. In the interest of confidentiality we show as little information as possible on our drawings; especially drawings that customers will see. I don't see that changing, although I think we may have to tweak the way we do things once everyone here starts using NX. I'm told there are some things that Ideas will do that NX won't, particularly in Drafting. I'm taking such comments as truth simply because I know next to nothing about Ideas.

It would be great if hidden lines could work the way I described in a future version but I'm not holding my breath. Even though it makes a lot of sense I'm sure it's nowhere on their radar screen as far as enhancements.

Mike

 

[hudson888]

Mike,

I can only advise you to use NX as the system was designed to be used not as some other system happened to accommodate. Otherwise you're just making a rod for your own back. We've given you a couple of options already and explained best practice, so the rest is up to you.

I can only speak for CAD systems that I know and if by offset you mean shell (formerly hollow) or thicken or simply offset surfaces then these geometries are all pretty much equivalent. If you create a design with any concave elements then there is going to be a point beyond which it cannot offset without self intersecting. NX does a good job of producing those offsets which are possible. You can't honestly blame the system when your model includes small elements that it cannot reproduce.

CAD systems are even getting to the point of selectively excluding elements that cannot included in solving how a shape is shelled out. They don't do everything but they do a lot.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Crocostimpy]

I'm not blaming the system(s) for not being able to shell the models, I just meant that because of our geometry we've never been able to do it. And it just so happens to work out that we don't really need to anyways. : )

Actually, at the place I previously worked they had Imageware (I think) software. It had come with the laser scanner they had bought quite a while ago back. That program would shell out our models very well. If it found a surface it didn't like, or one that would disappear because of the offset, then it would throw it away and approximate that area based on surrounding surfaces. It almost always worked very well. We used it to shell out models to make prototypes. I've been trying to put a bug in someone's ear about it here but these days no one wants to spend any money.

Mike