Hybrid Design

[UGMasters]

Hello,
I work for a company which produces Injection molds
for automotive Industry.I have done Hybrid modelling(Solid &Surface) on Catia.

We recently converted to NX in our design dept.How do you apply the same concepts with NX, or is it possible,if so
please elaborate.

Thanks
Girish.

 

[ewh]

Yes, you can do it. Depending on your requirements, you can use fully constrained sketches, paramaterized features, expressions, or just grab and pull your surfaces arount as needed. As for how to do this, you are going to have to refer to the Help files or get some sort of training. It can turn into a big subject because so many different tools are available to use.

"The ambassador and the general were briefing me on the - the vast majority of Iraqis want to live in a peaceful, free world. And we will find these people and we will bring them to justice." - [small]George Bush, Washington DC, 27 October, 2003[/small]

 

[hudson888]

Girish,

In NX you can build from Sketches for your basic extrusions and the creation of very similar sketch based solids to those which CATIA supports. However one thing that UG has which CATIA doesn't is the addition of several kinds of primitive bodies which can be booleaned (that means unite, subtract or intersect with one another).

There are features like pads, pockets, holes, bosses, slots and grooves which can be applied to almost any solid. In NX you can extrude a sheet or solid based on curves or the edges of other geometry, another thing which requires extra steps in CATIA.

Then there are feature operations based on existing geometry such as shells, and thickens, extractions of sheets or solids, scaling adding draft or blends and chamfers to name a few.

In NX you can create sewn solids from sheets, kind of like volumes in CATIA. You can also take an open sided sewn solid which matches another solid and Patch it onto the side to make a single booleaned solid.

NX support surfacing based on curves which is in many ways similar to CATIA. There are several edge and face to face blend types which can be applied to sheet or solid bodies without any real distinction.

Then there is Direct Modelling which provides a whole new set of tool to work on geometry without parameters but in timestamp order so that the direct modelling feature is parametric in itself. These are extremely powerful and great for overcoming poor modelling in older models. The tools are replace face, delete face, move region, offset region, pattern face, and constrain face plus a couple of others. The simplest example that explains its power might be to imaging a simple but fully blended model with no taper and NO parameters. This kind of thing that you'd have to rebuild to add taper for manufacturing, except that with direct modelling there is every chance that you can constrain the vertical faces to have taper and get the result you needed. Since it works with faces you can delete them but it can not recalculate the model in such a way as to add an extra face, so sometimes you still require a separate solution, but when it can work it is capable of doing things unthinkable in most other CAD systems.

NX-6 introduced synchronous technology which roughly described takes a step beyond Direct Modelling into uncharted territory. Its intention is to provide a toolkit for doing changes more interactively on the fly and without spending a great deal of time and attention on the parametric structure of the model. As I'm not able to get into it further than that since I haven't yet used it very much I'll just say that it is very powerful and I have seen nothing like it in any other CAD system.

The organisation of the features tree is one of the most different things between CATIA and NX. It will take some getting used to swapping in either direction. Users of CATIA V5 and NX find them probably more similar than CATIA V4 and V5.

Another main difference is that NX managers the display of altered entities differently in that when altered the original is not hidden or duplicated it can be simply replaced by the altered version. In many dialogs this is the default behaviour and it means that you have less hidden geometry to manage in your file. It is a more what you see is what you get approach. Yet for all associative features you can use the timestamp based feature tree to look at the feature as it was before an operation was applied in order to analyse how a model was built or simply go back and insert a feature before another one where necessary.

Anyway that is a brief overview. I'd very much suggest that you investigate some training. There are some courses about that cater for users coming from other systems who can skip over some basic steps to do with learning about 3D concepts etc. Try cast if you have it or simply turn on an advanced role to display as many modelling icons as possible, using F1 to display the help files will give you some idea of what each of them does as a good starting point for anyone prepared to self teach. Otherwise contact you local PLMS support staff for the training or you can also try

http://www.myigetit.com

where they have some basic online courses that you can purchase.

Best of Luck


Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Xwheelguy]

Trim Body is a fairly powerful command in NX, which I didn't see mentioned above unless my skim-reading is getting me into trouble again. Apologies in advance if I did miss it to those that have already replied.

Basically, if you have a solid body, you can create surfaces(sheets) and Sew them together to form a sheet body that could enclose a volume of the Solid (it doesn't have to completely enclose it, just extend beyond the solid's faces. You can then use Trim Body to trim away the solid using the sheet body. You don't necessarily have to enclose an area/volume either, depending on what you're trying to do or what the solid and sheet(s)look like and how they intersect. Try to avoid having your sheets converging tangetially into the solid...this can create issues (the dreaded non-manifold solid).

The NX Documentation should provide some basic examples that should give you an idea of what I'm trying to describe. Depending on what you're used to doing in CATIA, I'm fairly certain the equivalent modules (workbenches) in NX will be able to do the same thing, it's just termed differently.

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.

 

[UGMasters]

Thanks Guys for the help,
I am aready on it Synchronous modelling is great !!
I tried Trim solid fuction as well...I am getting there

thanks once again
Girish.

 

[jerry1423]

I agree with nkwheelguy in that "trim" is a very powerfol command.
"Replace Face" is very similar to that. It is differnt in the way that solid material does not have to be removed for it to work.
"Replace Face" is one of the original commands of UG Solids, but it wasn't until NX4 or NX5 that it became associative.