Sharing well constructed CAD models. 5

[SiW979]

Hello all

I want to start this thread to try and encourage people to perhaps share some cool parametric CAD models. Obviously I'm not talking about your company’s valuable data, but the models you may have created whilst practicing in your own time etc. I'm fortunate in that I am an NX CAD/PLM trainer so I spend a lot of time just playing with NX and learning new things that I can them pass on to our design engineers, so a lot of the models I create are nothing to with production machinery/sensitive data etc.

What I do know is that a picture, or in our case a model speaks a thousand words. How many times have you read a thread only to be lost in translation by the 4th line? Well, when ever the engineers at my company ask me a question about how to do something, I try and model it in native and email it to them so they can pick through the history and work out what is going on. I also save and keep as many .prt files that are posted here for reference. So to get the ball rolling I have attached a model of a parametric agricultural tyre. Try playing with the expressions; change the tyre diameter, the tyre width, the number of treads and the height of the treads.

One of my missions at work is to ensure that we all get the maximum return from out investment and that all divisions are working to the same level, and sharing information is a great way of doing this. You never know, you might just leant something new.

Enjoy...


Best regards

Simon (NX4.0.4.2 MP4 - TCEng 9.1.3.6.c)

http://www.jcb.com

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

 

[jerry1423]

I only had a little bit of time this morning to play with your model. It looks very nice and is well done, except that the number of threads cannot be increased, only decreased (if the other settings are kept as is). If the number of threads is greater than 11 it does not work.

Thank you for sharing this with us.

 

[mmauldin]

I tried increasing the number of treads up to 15 and it works for me. May work for more, I just haven't tried.

Nice model.

 

[ewh]

Thanks for an excellent suggestion! A company library with files containing common (and some not-so-common) situations and solutions can be a valuable asset.

"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]

 

[mmauldin]

This a template file I use for compression springs.

 

[jerry1423]

I wonder why it did not work for me? Maybe it's a tolerance setting. I got the error that three tiny objects were found. I am working in NX5.

Is it possible to get some sort of folder here that these files can be placed?

 

[SiW979]

Jerry

Note that being able to increase the number of treads is dirctly linked to the diameter of the tyre. If the tyre diameter is small e.g. 700mm then you will be able to fit less treads on it than if the tyre diameter if large e.g. 1250mm.

Best regards

Simon (NX4.0.4.2 MP4 - TCEng 9.1.3.6.c)

http://www.jcb.com

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

 

[SiW979]

Here is another model I use when training people how model parametrically. It maybe familiar to some of you as it used to be used by UGS as an additional project at the back of the Practical Applications manuals.

I use it to show the power and benefits of using reference geometry for positioning features and also how to link one sketch to another.

It's also an excellent example of how careful one has to be when applying constraints, so many of my trainees have concentrated on ensureing sketches are fully constrained and when I ask them to make a change, the model falls over instantly because fully constrained doesn't necessarily mean well constrained.

I've also added some extra features that are suppressed by expression which are really useful if you work with part families etc. Play with the two named expression in the expression editor, they are currently both set to 100, but change them something under 100, but not less than 57, that's as low as you can go before blends start to intersect. Notice that when you go below 100, the 10 large bosses become 6 and the 7 small bosses become 5.

Perhaps if John Baker could get permission, he could post the drawing on line too so your young/inexperienced engineers could have ago and use this model as a benchmark.

Enjoy...

Best regards

Simon (NX4.0.4.2 MP4 - TCEng 9.1.3.6.c)

http://www.jcb.com

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

 

[JohnRBaker]

Simon,

While I can't vouch for where the course-ware people got their inspiration, I also used this example for my NX 6 testing earlier last year and I've attached a scanned image of the document which I used. Now there are some subtle differences, but there's no question that the model you downloaded is a direct heir to the one I used.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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]

John

Many thanks for posting the image, I have attached the same one, albeit in metric obviously to cater for the european users.

Best regards

Simon (NX4.0.4.2 MP4 - TCEng 9.1.3.6.c)

http://www.jcb.com

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

 

[adrag]

This is an excellent idea. I've downloaded the models, played around with them a little in my (limited)spare time, and already learned a thing or two.

Simon, I have a question on project22. How do you parametrically suppress objects? For instance, on boss(18), when I bring up the information window, I see that p175 is the suppression state and is defined by an equation that suppresses the feature when the width is less than 100. If I were placing a new hole or boss on my model, where do I enter then suppression state? Thanks.

Al

 

[jerry1423]

adrag ...

I have not had time to look as closely as you have at the models, but I assume that he used "suppression by expression" for what you are speaking about.

In my opinion that is one of the most under-utilized things in NX CAD and is very useful. It would be worth looking it up under "help".

 

[SiW979]

Al

Go to Edit > Feature > Suppress by expression. This will allow you to apply expressions to features you have created either in an individual basis or by creating a shared expression. There are two status that the suppress by expression can be, 1 (on) or 0 (off) so in my model p175 will probably read something like: if main_rad >= 100 then 1 else 0.

So as soon as you make the main rad anything under 100, the the suppress by expression status goes to 0 which suppresses the features.

So simple yet so useful and under used as jerry said. I'll try and post another example soon.

Good luck!

Best regards

Simon (NX4.0.4.2 MP4 - TCEng 9.1.3.6.c)

http://www.jcb.com

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

 

[jerry1423]

You can also supress components in an assembly by expression.

 

[adrag]

Thanks again. This opens up all kinds of modeling possibilities for me. Great thread guys!

Al

 

[SiW979]

Using deformable parts.

Many people use proprietary parts in assemblies, in this post I will be using a gas spring as an example, to the manufacturer of the spring, it is an assembly of parts, however to us we consider it as a single part and as such usually create a single solid simplified representation or space claim.

However the a gas spring is a dynamic component and we would be interested in the closed and fully extended positions, but don't necessarily want to model an assembly with arrangements to show the closed and extended postion.

This is where deformable parts come into their own. Open the part I have attached to this post, as you can see it is a gas spring/strut. Analyse the model, notice how the sketch has been constructed and more importantly notice that there is a parameter that has been named 'stroke' which has been set at a 300 or the closed length. This expression will by the basis of the deformable part.

Have a look at the last feature in the tree, this is the deformable feature, you can't modify this, if you wanted to change anything in the deformable part, then in NX4 you would need to delete the feature and run through the deformable part wizard again.

Now create a brand new empty part. Add the gas_strut1.prt to the new part suing assemblies, simply accept all the defaults by clicking OK, to all dialougue boxes, however, notice that there is an extra box at the end with a drop down menu with 2 values in it (300 and 490) relating to the parameter stroke. You could define either or, but in this case accept the default of 300. and add the part.

Now look in the part navigator (not the assembly) you will see a single feature in there which is the deformable feature. Double click this and change the value to 490, notice that the gas spring length grows to the fully extended postion. Now make the gas spring the displayed part by right clicking in the assembly navigator. See how the gas spring has not changed in its own file, only in the assembly where you have added it. One of the nice things about this is that it works with mating conditions so you can simulate a door opening and closing for example simply by changing the deformable value.

To create a defomable part, go Tools > Define Deformable Part> and work through the wizard.

Tip when it asks what you want to add to the deformable part, just select everything. On the expressions page select the single expression you named such as 'stroke' in my example. Carefully thought out models are a must to ensure success.

Enjoy...

Best regards

Simon (NX4.0.4.2 MP4 - TCEng 9.1.3.6.c)

http://www.jcb.com

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

 

[hudson888]

Simon,

I seem to remember that tyre I learned with you on that one and repeated the tricks for the um "Leap Year" version on the website!



Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[SiW979]

Hudson

Yes, you did help me on a tyre a while back, I've been practicing hard since then and have learned a hell-of-a-lot since then about building decent models with anticipated changes might take place. The tyre in this thread is a brand new one, the one we did was as much use as a chocolate coffee pot as there was virtually no scope for modifing parameter without it falling over.

Like the image by the way, are you working in Oz nowadays? I thought you were in the states?

Best regards

Simon (NX4.0.4.2 MP4 - TCEng 9.1.3.6.c)

http://www.jcb.com

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

 

[ZeissMetrology]

I am often asked by our potential customers if our CMM software can make sue of NX 5 CAD models with embedded GDT. The answer is Yes but I am seeking some simple example .prt files to demonstrate this. Does anyone have a file to share with the GDT embedded? Thanks so much.

 

[potrero]

JCBCad,
Thank you for sharing the gas_strut model. For some reason, the expression in the assembly file controlling the length of the extension is actually showing up as "Horizontal_Dimension_between_Arc3_and_Arc2_17" instead of "stroke". Is this what you're seeing too?

Also, for deformable parts, can you allow for a range of values, say, between the min and max stroke?