Define Variable 8

[LucasBam]

I am using Law Curve to define a sine wave
I then want to wrap the sine wave around a cylinder
It will wrap around but the length does not match the cirecumfrance

I assume I have to define t as a varible from 0 to the circumfrance, does anyone know how to do that or if there is another way to do this

Thanks Luke

 

[JohnRBaker]

What version of NX are you running?

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.

 

[JohnRBaker]

Assuming that you're running NX 3 or a newer version, here's an example of a Sine Curve in which you can edit directly the length of the final curve. Note that this model is in Imperial Units (Inches), but the expressions would be the same.

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.

 

[jerry1423]

The wrapping about a cylinder is the tricky part of this problem.

I really enjoy problems like this, and personally I get so caught up in them that I may work many hours on something that should have taken a very short time by doing it another way.

You may just want to use the "wrap/unwrap" command under "curves" to get the sine wave to wrap around a cylinder.

 

[mmauldin]

This is a slight edit to John's model. It calculates the length directly from a diameter varible.

 

[man2007]

Hi Luke,

hope following part answers ur question.

 

[man2007]

Well, the equations used in the above part are 'modified version' of the so called "Toroidal Spiral", see the following attachment

 

[LucasBam]

Thanks, the equations and the wrap command worked and I now have a sine curve around a cylinder.

I want to use it to cut a cam groove out of the cylinder, I have tried various swept/sweep commands with no real sucsess, any ideas?

Thanks

Luke

 

[jerry1423]

Maybe try extruding it. Make sure that all of the menus are open under "extrude" so that you see where you can extrude it in two dimensions so that you get the depth of the groove as well as the width.
I really am not sure if that will work and you may need to play around with it a bit to get what you want.
Be sure to take note of the direction of the extrude (shown with arrows) so you can either change the direction of the arrows, or enter negative values, to get what you want.

 

[hudson888]

LucasBam,

The short answer in two words is Law Extension. This was one of the parts that ribbon surface didn't seem to do so well with.

The technique would be to create a surface and then using a series of thickens trims and offsets you will be able to create a groove that is probably what you would expect. See the attached part.

There is another alternative that says you simply wanted to make a fancy oil groove of sorts. For that you'd simply create a tube using the spline that Luke kindly provided then subtract it from the cylinder. If that's all you needed then good luck and ignore the rest of this post.

Now caveat emptor because this is probably really only what you think the model should be like. What I'm guessing you might want to do is machine this with and end mill or slot drill probably on a CNC machine with a 4th Axis. If I'm right it probably operates as a lifting cam with a pin in the slot. You only really need the cylinder and curve to create a program and the result will be most suitable to your needs. Surprisingly enough the model that I've supplied isn't always exactly 100% accurate. Something I found out when we once conducted just such and exercise and compared Vericut output used to check the program with the geometry we assumed to be correct.

The answer is that the swept volume of the cylindrical cutter scavenges a little more material off the sides than you might expect and neither is the bottom of the groove perhaps quite as cylindrical as you might expect. I know of no really practical way to correct these what are after all minor modelling discrepancies because NX won't allow you to sweep a solid. Nor does it really matter for any known practical reason. We only found it by accident and it remains one of the few geometries that sticks in my mind that we couldn't readily produce using NX modelling. I'd add that I don't know of any system that would do it but sneakingly hope to be proven wrong someday!

Of course the latter part of this is just and esoteric examination of a particular observation that I thought was cool but heck what can I say. I'm hooked on geometry. My excuse is that it's what I do!

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[mmauldin]

I find myself using a lot of circular cams in my work. I usually use the technique shown in the attached part. It does require a little extra work (drawing/wrapping a second guide curve) but the results are pretty close to the desired geometry.

This would be a nice enhancement to NX's capability. Add the ability to extrude/revolve/sweep/etc. a solid body as the section, similar to the way NX Machine verifies toolpaths.

 

[potrero]

mmauldin,
How did you go about inserting the numeric Notes on your cylinder body? How do you edit them later?

 

[mmauldin]

They are done in Drafting with View>Display sheet turned off. Once the display sheet is turned off, you use the standard Text command to add the text. The text is placed on the current X-Y plane of the WCS, so you have to set the WCS to match the desired orientation of the text. Transform can be useful when rotating when doing multiple text around a cylinder.

Editing is simply done by double clicking on the text.

 

[JohnRBaker]

You can also use...

Insert -> Curve -> Text...

...to create actual geometric curves representing a text string which can be added to your model like any other curves and used as such, including for creating features, like raised letters or embossed text. And since these 'text strings' are a feature they can be edited changing the text and having the curves update.

In the attached example, go to the Part Navigator and double-click on the Text feature which I've renamed "Edit Me" and edit the test string and hit OK.

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.

 

[potrero]

Thanks for the info and the examples.

 

[SiW979]

Hello there

I wonder if anyone would be kind enough as to tell me what exactlly 't' is and how it applies to a curve etc? it jsut seems a little odd that 't' can equal zero and 360*t will = zero, so what is the point of that part of the equation?

I warn you now, you are speaking to a non-engineer so keep it simple (reasonably) or I my brain may subjected spontaneous discombobulation.

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...

 

[cowski]

JCBCad,
refer to

http://mathworld.wolfram.com/ParametricEquations.html

 

[mmauldin]

As i understand it, "t" is a built in variable used by NX. While you are required to add the expression t=0 (or t=some number), in actuality when "t" is used in an expression, the expression is evaluated for all values between 0 and 1.

 

[JohnRBaker]

Think of 't' was being the range of an integral, which in this case is from 0 to 1.

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.