Sharing well constructed CAD models II 8

[SiW979]

thread561-234523

Sometime ago I created a thread trying to encourse people to share their we constructed CAD models so that others may play around with them an possibly learn a trick or two.

Anyway the thread has been closed, but a reference to it is at the top of this one. I've got another CAD model here of a piece of round tube with a sqashed flat end,which one of my users aksed me to show him how to do, so have a look and see what you think, I'd be interested to see other peoples interpretations and also critiques of mine.

For anyone who never saw the original thread, I would recommend you have a browse through some of the excellent CAD models that people posted on there.

Enjoy I

Best regards

Simon (NX4.0.4.2 MP10 - TCEng 9.1.3.6.c)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[michaelmould]

Guys and gals,

This is a great thread! Perfect for me as a relative new comer to NX. I'm just starting to use expressions and things in my work, so the working examples shown here, along with the technical information are invaluable.

Just wanted to post a message so that the thread didn't get lost again, it was about to fall off the front page!

Does anyone else think creating a forum for this topic alone would be a good idea? With each model and subsequent comments being an individual thread. Just a thought.

Thanks again for the invaluable lessons!

Mike

NX6.0.3.6

 

[SiW979]

Hello all

I don't think I've posted this one before, but it's quite a cool model. Bascially the pitch of the blades is controlled by one expression. So open up the expression editor and play about with the OUTER_PITCH and see how this effects the behavior of the model. I think the max it goes to before a blend fails is 82

Enjoy

Best regards

Simon (NX4.0.4.2 MP10 - TCEng 9.1.3.6.c)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[Andy512]

I like that one. Wish we had a studio license as I am guessing that's how the mirror effect was accomplished?

 

[cowski]

The mirror effect is a type of face analysis called 'reflection' and it can be done without a studio license.

 

[JohnRBaker]

I may have posted the Imperial version of this file before, but I've since created the Metric version so here are both.

I'm talking about a 'Wave Washer'. These models shows off the use of such functions as Law Curve, Wrap Curve, Instance Geometry, Thicken, etc.

In both of the attached files you can edit the Inside/Outside Diameters as well as the Thickness of the material and effective Thickness of the washer by going to the Part Navigator and expanding the 'User Expression' section, double clicking a parameter and entering a new value. I've also included a pair of Datum Planes (representing the top and bottom 'faces' of the effective height of the Wave Washer) which will make it easier to Constrain the Washer in an Assembly. You can use the 'Y' Axis of the Datum CSYS for alignment.

Note that both models are in NX 5.0 format so that should help those who have not yet moved to NX 6.0.

Anyway, give them a look and have fun.

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.

 

[SiW979]

Andy 512

Have a look at the attached .avi file which will show you how to add face reclection. Hope it helps

Best regards

Simon (NX4.0.4.2 MP10 - TCEng 9.1.3.6.c)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[RobLN]

Hi JCBCad

That reflection command is pretty neat. Any way to apply it to different components in an assembly? Seems that if you select one of the parts with reflections on the other components go into wireframe mode.

Also if you apply the reflection to the component then open the assembly where the component is used the reflection does not follow.

Rgds Rob.

 

[SiW979]

Hi Rob

Whilst reflection is a nice way to make components look glossy and slick, this is not the main function of the command, infact it is pretty much unintentional. The relection tool is actually an analysis tool that is used by people who want to create very high quality surfaces with out any mismatched edges or unintentional inflections or imperfections in the surface.

For example any one creating the a surfaces of a car would use this tool to make sure that light flows smoothly over the surface of the car.

We've all done it ourselves, we go to buy a nice new or second hand car that's clean and shiny and you find yourself crouched looking along the sided of the car for dents in the pannels, obviously with a bright light or the sun shining on the body pannels the dents stand out very easily, and that is basically what this tool is for, checking the quality of sufaces, the fact that you can make you model look more realistic for presentations etc without having to know how to create a full bore rendering is just and added bonus.

Have a look at the attached model, spin it round an notice where at the point where some of the sheets meet, the zebra stripes are not contiguous and they don't flow smoothly, if I was a good surface modeller (I'm not, hence the poor quality) I would be most displeased with this model, they should flow smoothly, if you have one of those iPODs with the chrome back, look at the reflection of something stripey in it and see how perfect the surface is.

Best regards

Simon (NX4.0.4.2 MP10 - TCEng 9.1.3.6.c)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[SiW979]

Hello people.

For those who are on slightly older versions of NX like me who still need to use datums in order to put holes through a curved surface, I have attached a model which will hopefully show you how you can create a hole which pierces surface normal to the face regardles of what you do to the controling expression. Suppress all the features and look through them one at a time.

The important bits start with the HOLE POS sketch consisting of 1 single reference line. The length of the line is controled by a named expression called PCD.

I exited the sketch and added an associative point ot the end of the line and then projected that downwards normal to the surace of the revolved face. I then added another datum (type: point and direction) using the 2 poiint option of the drop down menu within the datum command and the associatice and project points to define the plane normal.

Then simply add a hole to the datum and position it point onto point of the projected point and create your circular array.

Open the expression editor and modify the PCD expression between 300 and 60 and notice that the hole will always be normal to the face.

Enjoy.

Best regards

Simon (NX4.0.4.2 MP10 - TCEng 9.1.3.6.c)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[Andy512]

Simon,

Thanks for the tips and models.

Never knew it would do this.

Just goes to show what you can learn this software will do by getting outside of your usual methods and practices.

 

[mmauldin]

Since we are having fun with law curves let me throw one onto the pile. A while back I needed to represent a "BalSeal" spring and quick Google search turned up the formula for a toroidal helix. This became the basis for the included law curve.

The "p" value in the expressions controls the number of "strands" in the helix.

While the "q" value is a formula, it can be directly input as an integer and controls the number of coils.

Adding a multiplier to the formula for "zt" causes the model to take on a squished appearance. Use a multiplier greater than 1 to flatten the coils in the x-y direction, less than 1 to flatten in the z direction.

 

[RobLN]

Hi

Here is a spring I created with law curves. I am trying to make the spring adjustable. It's by no means perfect but it meets my requirements.

I've also played around with linking the spring expression variables so that when I change the position of items in the related assembly the spring compresses / extends. This theory works great until you need to create 2D separate views of each position!

Such a shame that arrangements is not compatible with the assembly constraints...

If anyone can model the part in a simpler way I'd be interested to see the method.

Note model created in NX V5.

 

[SiW979]

Hello people

Here is a cracker for you, perhaps a little more interesting to anyone who is involved in surface modelling, although it does make pretty good reading to anyone. It would be good point of reference.

Enjoy.

p.s. whilst I'd love to take the credit for creating this beautiful model I can't, because I didn't do it. :-(

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[mmauldin]

RobLN,

I modified a spring I submitted on the last model sharing thread to allow for controlling the number of closed coils.

While it is constructed as a deformable part, I have found that the deformation occasionally behaves erratically when placed in an assembly.

 

[hudson888]

Simon,

Nice work if you can get it! Probably you wanted to loose the reference data out of that file. I'd love to know what the intention was in relation to the STL data. It looks more like old sheet metal off CAD than a scan off clay perhaps.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[RobLN]

Hi Mmaudlin

Thanks for posting the latest version of the spring. Thats what I was looking to achieve but your model is so concise. I like the addition of the 'closed coils' into the base sketch. Simple & effective, nice.

Now we all of the benefit of how to do the spring - and how not to with my attempt!!

 

[SiW979]

Hudson

Siemens used a data set of one of our machines to launch NX5 some time ago, we also asked them to come in and demonstrate Shape Studio to our ID team with the intention of binning Alias and unifying all our CAD data under the Siemens umberella. So they took a translation of the Fastrac boonet (already a production part created using crap alias to nx work flow) and then used this to re-model the bonnet associatively using shape studio to show how quick models could be updated compared to Alias. Hence all the reference geometry. ;-)

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[man2007]

Recently I created Spring with closed coils, using Law Curve. Following Spring Parameters can be varied:

1)MEAN DIAMETER OF SPRING
2)WIRE DIAMETER
3)FREE LENGTH
4)NUMBER OF ACTIVE COILS
5)TOTAL NUMBER OF TURNS

 

[kukelyk]

Simon, in the profile_2 file the sketch dimensions are visible, even if you are not in the sketch. How did you set it?
thanks in advance

----
kukelyk

 

[RobLN]

Hi Man2007

Thanks for sharing that excellent model with us. Here is a metric version. Adjust expression values to suit. -currently its a very small component





Solid Edge; I-Deas 7 to 12; NX4 & currently NX5.