How can you model this part in NX5? 6

[RobLN]

A general question here, I'm having a hard time working out how to set up a sweep to get a part like the one attached below.
Any advice greatly appreciated.

 

[speedster29]

I would take a look at it but I cannot open your file.

 

[JohnVincent]

Here is a real basic example, it's hard with out any parameters given on this feature. There is better ways if you give more information on the part.

 

[RobLN]

Hi Speedster sorry you can't see the file. Maybe you can look at the file attached by JohnVincent he has the file I sent in the .prt file.

Hi JohnVincent thanks for the pointers I'll play around wth the project curve command to see what I can get. At least I know where to begin now...

 

[JohnRBaker]

OK, here's the approach that I would take.

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

http://www.siemens.com/plm

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

To an Engineer, the glass is twice as big as it needs to be.

 

[hudson888]

RobLN,

Have a look at the attached because there is more to be understood about such examples than may at first meet the eye.

I suspect that what is really involved is that the groove would be cut using an end mill on the 4th axis of a machining centre. It creates a geometry for which the perfect swept solid path is difficult to define. My first example more or less arrives at a construction method attempting to duplicate that kind of geometry. It looks rough and more like the original. The second example is more or less like what I think John has modelled in NX-6.

Delete the Move Face at the end to overlay the two. Sorry if the features are a bit of a mash it really isn't such a complex design anyway. In all likelihood you may wish to differently constrain the wrapped sketches. I didn't bother since it wasn't necessary to prove the method.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[RobLN]

Hi John & Hudson,

Thanks very much for the support on the model side. that really gives me some ideas.

Sorry John, but I can't open the NX6 rev file. Would it be possible to convert to NX5 please?
I would like to take a look.

 

[hudson888]

RobLN The second version in my file was exactly the same method as John's except that he may have constrained the sketch properly and really that part IS up to you.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[mmauldin]

Here's a slightly different take.

 

[RobLN]

Hi Mmauldin - thanks for your input. I've learnt a great deal form looking through the history tree. Thanks for taking the time.

 

[JohnRBaker]

RobLN,

What version are you currently running? I've got another idea that I'm going to try out which might be closer yet to what is desired, but I want to make sure that you can see the final model.

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

http://www.siemens.com/plm

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

To an Engineer, the glass is twice as big as it needs to be.

 

[RobLN]

Hi John I'm running NX 5.0.4.1 (on windows XP)

Look forward to seeing what you come up with!

 

[mmauldin]

What's really needed here is the ability to sweep a solid, i.e. a cylinder that would represent an end mill, along a set of guides. This would be very helpful in constructing a model that accurately depicts the result of milling a spiral slot. I have had other instances where creating a model by driving a tool along a tool path would have made my life much easier. Future enhancement, maybe?

 

[JohnRBaker]

RobLN,

One other question, are you working in Metric or Imperial units?

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

http://www.siemens.com/plm

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

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

OK, assuming that you're working in Metric, the part attached to this post is an NX 5.0 version of what I modeled the first time in NX 6.0, but I don't think it quite does what you want although it comes very close and it's very well behaved and it only took 9 features (not counting the Datum CSYS).

However, in my next post I'll include a slight variation which I suspect is what you're actually looking for.

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

http://www.siemens.com/plm

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

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

Now this is my second try, which I suspect will be much closer to what you're looking for, however this model required 12 features (not counting the Datum CSYS).

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

http://www.siemens.com/plm

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

To an Engineer, the glass is twice as big as it needs to be.

 

[SDETERS]

I am not an UGNX user but try to follow the way I would model it In I-deas. (Maybe you can model something simliar in UGNX. First I would create surface that follows the centerline of the cutter. (OK I-Deas Command here do a surface Offset) of that surface and do not keep the orignal.
Model the same surface and do a surface offset of that surface to the other side opposite of the first surface you made. The surface offset equals your cutter radius. Cut the ends off with an extrude where you want your tangent of the cutter to end up at. Make a flat surface at the ends you have cut. Do a (I do not know if UGNX has this I-Deas has all of the perfect commands LOL) Three Surface Fillet between the three surfaces. Now you have the geometry you need.

 

[hudson888]

There are now so many possible results to this problem that you probably have to ask yourself which could be right.

I have attached the little assembly that I have created to illustrate a few of the earlier examples as compared with what I have found later on.

Mike Mauldin is right in saying that a swept cutter is difficult to duplicate. The thing that he's probably not going to believe is that the swept method he used produces nothing like the correct result. I have subtracted a series of tubes from the solid body to approximate an actual cutter path assuming that the machining method is indeed a 4th axis milling process. I think we can safely stick with this because the original geometry bears it out.

The closest results to the actual sides of the slot were obtained using examples which created a law extension sheet, thickened it and then subtracted. The bottom however wasn't very close at all.

In the latest example number 3 I have used the law extension surface and some wrapped curves to sweep a section using no less that three guides AND a spine curve to control the shape. This is interesting because although some of the surfaces are still quite rough in a few places there is a close match between both the original step data and the section of pseudo cutter path.

I don't know if anybody is really going to take this much interest in the question but it is interesting for me because in an earlier version we attempted the same thing and found ourselves stumped by such an example. I think this time we're a little closer if anything.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[mmauldin]

"The thing that he's probably not going to believe is that the swept method he used produces nothing like the correct result."

I have no problem at all believing this because I have been down this path many times before. For creating a general depiction of the part this doesn't pose much of a problem. As for drafting, I use curves to describe the center of the slot along with a depth/width callout. The biggest problem I run into is when our manufacturing group tries to use the model with a CMM to verify the part. That is why I would really like to have a way to sweep a solid along a guide.

"The closest results to the actual sides of the slot were obtained using examples which created a law extension sheet, thickened it and then subtracted."

Granted, but using a cylinder to create the end condition gives a much more accurate result for that portion of the feature. Perhaps a hybrid approach would be the best overall solution.

 

[mmauldin]

"Hybridized"