helical sweep in NX4?

[66gto]

In NX4, every time I try to sweep a section along any type of curve, the section twists along the way in an unexpected way, and I get a weird twisted solid. It's been a few versions ago since I've been at a CAD terminal regularly, so either I'm dreaming, or it used to be really easy to do a swept section along a guide in previous versions of UG.

Right now I'm trying to sweep a simple triangle section up a helix, such that the triangle section turns along the helix (i.e. the inside point of the triangle always stays on the inside for one full revolution. Any suggestions on how to approach this?

Thanks.

 

[JohnRBaker]

You need to define something that will align your model as it is swept along the helix. Lets assume that the axis of the helix is aligned with one of the principle axis of the current WCS (if it isn't just move the WCS so that it is). Now after selecting the helix as the 'Guide String' and the triangle as the 'Section String', continue to hit OK until you get to the dialog where you're asked to "Choose orientation method". Select the 'Vector Direction' option and then select the appropriate 'Vector Constructor' from the list of possible cases. Now hit OK a couple of more times and you should have it.


John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

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

 

[cowski]

The vector that you want to pick is the axis of the helix.

 

[66gto]

Awesome, thanks Cowski! I was struggling with John's tips and still couldn't get it to work, but you provided the key. Works great now, thanks to both of you guys!

 

[Xwheelguy]

John,

Somewhat off-topic, somewhat on-topic:

Given that it's obvious (at least to me) that new users constantly struggle with what are simple Sweeps in competing softwares, are there any plans to revamp the current Sweep command in NX so that the user can expect to get the oriented sweep like the above? If not, then would you feel it would be such a bad idea to break the Sweep command down a little further....or should I ask how would UGS development feel about that?

I understand the need to have multiple types of Sweeps, or the additional options, but it appears to me that many users struggle to figure out that magic little trick of choosing the correct orientation. Maybe come up with a new Advanced Sweep that allows for all the other sweep types or choices but make the current FFF Sweep the feature that does a little more assuming or as simple as possible as far as the orientation is concerned.

I rarely see novice CATIA users struggle as much with the Sweep command compared to NX, and there is far less interaction with the dialogs as well. Yes, I know the dialogs are changing in NX but it's not really the dialogs that introduce the confusion, but more along the lines of what is required user input in order to produce a final shape. I guess the real question is could the whole Sweep definition (for simple sweeps only) be simpler for situations like above in NX or is it as simple as it can get the way it is now?

Not bashing or criticizing, just throwing around ideas based on experiences with other softwares

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[JohnRBaker]

Well for NX 5 we have rewritten the UI for Free Form Swept feature, but we have not changed the way it works. However, the interaction is more consistent with other features, such as selecting the section string(s) first and the guide(s) second. And while it is true that we have not added any significant enhancements to the function itself, we have taken all of the options and settings and exposed them on a single dialog that will better show the user what can and/or needs to be accounted for. And since we have implemented 'Dialog Memory' any change in options will be remembered from one use to another (even across sessions) and so the options that are used most often will tend to already be selected. For example, out-of-the-box, both now and in NX 5, the default orientation is 'Fixed' which does not required any action, but as you say, it also doesn't give the desired result. While that's only an opinion, if it's true that Defining a Vectored orientation would be a more useful default, in NX 5, if during my previous use of this command I used the 'Vector Direction' Orientation method, the next time I use this command it will not let me continue until I either select a vector refenence or I change the Orientation method to something else. Granted, this is not exactly what you were looking for, but I think with the use of Dialog Memory users will tend to get the impression that the system is working closer to the way they wish to use it, even though what it's really doing is just remembering that often people use the same function, even one with many options, in a similar manner over and over again and this should help leverage that situation.

Now longterm, all of these complex surface/free form functions are being reviewed for seriuos and more fundimental rearchatecting, but for now, we're trying to get to a certain level of consistency first and then we'll work on the more detailed aspects.


John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

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

 

[cowski]

Will the swept command get a preview (or maybe it already has one, I'm still on NX2)? It would be nice to play around with some of the options before committing to the OK button (and having to redo all the picks and options if it isn't what was wanted).

 

[JohnRBaker]

While the long term goal is to eventually provide the ability to preview all modeling operations, that is not always possible, at least not yet. For NX 5, while we have made changes to the UI for most all of the modeling operations, even those where much work was done, preview was not always possible or pratical. In most of those cases, incluindg Free Form Sweep, we have provided an alternative that will allow you see the completed operation without losing any of your settings. In the dialog section titled 'Preview' where most functions will have the 'Prview' option, usually already toggled on, there will also be an icon labled 'Show Result' which will actually exectute the modeling operation but will not close the dialog. You can then either select OK, if the result is as you expected, or selecte the Icon a second time (which is now labled 'Undo Result') if it was not what you expected and you can then make any changes that you wish and re-preview the results until you get what you want. Note that even those functions that support full dynamic preview also have this 'Show Results' button. This basically replaces the old 'Confirm Upon Apply' mechanism that we have used with some modeling functions in the past.

Granted, this 'Show Results' may not be as nice or as efficient as a true dynamic preview, but it does provide some of the benefits and it is being applied in a more consistent and broadly available manner than when it was the old 'Confirm Upon Apply' which you had to trigger at the start of the process whereas now this option will become available when the system is able to perform the operation at the same time the OK button goes 'Green'. And over time, we will continue to add, in addition to the 'Show Results' a true 'Preview' option, to as many modeling operations as possible.



John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

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

 

[mjcole]

John,

Have there been changes to the Align by Points option. I remember struggling with this once while doing a complex sweep with 12 sections and having to pick blend point one for each section then pick blend point two for all sections and so on. I had to set up a screen layout to do this efficiently but even then it was annoying. It would be nice if these could be defined for each section and have the point numbers shown on screen for each section.

Michael

 

[JohnRBaker]

In NX 4 we added a very limited means of controlling Alignment Point for Free Form Swept surface, but a much more usable scheme was introduced for Surface Thru Curves.

In NX 5, we have taken what we did for the NX 4 Surface Thru Curves and implemented a similar scheme for BOTH Surface Thru Curves and Free Form Swept. What it does is automatically create a series of points, based on the shapes and number of curves in each section. These 'points' are displayed with a sort of rubber-banded line connecting the points on each section with the corresponding point on the next section. And while in this 'point alignment' mode, the user is allowed to drag the points along their part of the section curves so that you can define the exact alignment you desire. I think this will go a long way to make this sort of control more usable and should result in more predicatable model shapes.


John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

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