Defining Helix Law Curve(s)

[mycon73]

Hi,

This partially in reference with my, "Create Spiral Groove" topic. I need to create a spiral pattern to use as my sweep guide & the Helix curve feature seems to be the best feature to use.

I have start & stop points, ID & the # of turns required that will define my groove pattern. Other than these, I don't know what else is required to get the proper spiral pattern that I need. How & where do I difine Law Curve specifications & assure that my spiral pattern is on center with my axis that I'm going to make my sweep with?

Is there another curve option available to give me a defined spiral pattern?

Thanks




Jason Misztal
Fuel and Utility Systems
UG Designer

Goodrich Corp.
Rome, NY

http://www.goodrichrome.com

 

[joycejo]

Jason,
I did something like this a while ago. When defining the Helix one of the options is Radius Method - Use Law. I created a sketch to define the outline of a spring with two diameters. Then for the transition used a bridge curve from one dia to the next. I used these curves as the Law Curve and a curve in the center as the Base Line.

ftp://images.myigetit.com/spring_law_controled.prt

Right click on the link and select Save Target As to download the part file

ftp://images.myigetit.com/law_spring.gif

John Joyce
joyce@myigetit.com

http://www.myigetit.com

 

[abeschneider]

Jason,
A while ago I asked a series of questions about parametric helix creation, and John Baker gave some really informative answers.

You might be interested to check out the thread at:

http://eng-tips.com/viewthread.cfm?qid=164528

 

[mycon73]

Hi,

Received a lot of good suggestions, but for some reason, I still cannot get the Helix profile in a desirable location or get a clean sweep out of it.

I projected the curves as suggested, but when I go to create the Helix Law Curve, I'm not sure which one to pic for my needs. So far, none of them seems to be working for me. It's probably user error, but more guidance would be appreciated.

Perhaps, I can send a pic here. How do I include a pic with my topic?

Thanks


Jason Misztal
Fuel and Utility Systems
UG Designer

Goodrich Corp.
Rome, NY

http://www.goodrichrome.com

 

[cowski]

A picture would be useful. If you follow the 'process TGML' link (right above the 'submit post' button) it will have instructions on how to post images along with many other formatting tags. The tricky part will be getting your image uploaded to a web server. If your company has no such provision you might want to try a photo sharing site (such as photobucket). Many companies frown on posting of 'confidential' info, so be careful what you post - if anything. If need be, we'll do our best to work with written descriptions.

Use the tag to show images from any web server. Be sure to use the entire url to the image you want to use including the "[URL unfurl="true"]http://"[/URL]
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[hudson888]

Jason,

You create the taper helix per normal except that for the radius method select use law and input the top and bottom radii. I just measured the radii. The easiest way is if you place the WCSYS at one end of the bore with the Z-axis pointing along the bore axis.

I'd refer you back to the original topic for the full answer. I didn't think that projecting along surface normals was the correct solution because the top of the helix projects at the taper angle falling below the top of the bore.

Regards,

Hudson.

 

[mycon73]

Hi,

Since, I am blocked from various image sites, I will try to spell out my delima.

I have defined 2 points.

One point has a radius of: 4.828, which is my starting point.

The other point has a radius of: 5.084

If a line is drawn connecting the 2 points, this will represent my tappered face or ID bore.

The length between the two points is: 10.24

I believe I need to create a Helix feature with its tangent points along the tappered face & will start & stop at the specified points.

After I can be my Helix provile correct, I have my groove pattern that I will use as my cut tool, which is at a slight angle.

How do I prevent the cut from thickening as it sweeps around the Helix?


I hope this is sufficient info. for someone out here to assist me.

Thanks again for the assistance.





Jason Misztal
Fuel and Utility Systems
UG Designer

Goodrich Corp.
Rome, NY

http://www.goodrichrome.com

 

[kevklem]

Jason

1. Use your two circles(from the radii mentioned) to create a cone surface. The axis of which is your +ZC.

2. If needed rotate XC around ZC to the correct start or clocked position. Create a helix curve with a radius of 6 and pitch of 10.24 for one full turn. If you want two full turns use 5.12 for pitch. Note that the helix will begin on XC of the WCS and end on XC if using full turns.

3. Hudson888 was right on not using "Along Face Normals" as it does not give the right result. Instead, create a simple line at the axis of the cone surface. Use Curve Projection and for the Direction method, select "Toward Line" and use the simple line. The new tapered helix will start and stop at the same "clock" position as the parent helix.

Kevin

 

[kevklem]

When sweeping, set up section string normal to the end of the new helix string. For sweep orientation, choose "Another Curve" and select the original straight helix. When prompted for "Spine Curve" select the simple line on the axis of the cone.

Kevin

 

[mycon73]

Hi,

I finally got my Helix profile the way I want it - along the tappered face. For the most part, my cutting or groove tool sweeps well, until it gets near the end. How do I prevent the cutting tool from angling or thickening as it sweeps around the Helix?

Thanks....

Jason Misztal
Fuel and Utility Systems
UG Designer

Goodrich Corp.
Rome, NY

http://www.goodrichrome.com

 

[kevklem]

I guess I would add a second section (same shape) string at the other end normal to the guide string. Just be sure to pick the section strings the same. You will see a directional arrow appear when completing the string, make sure all the section strings have the arrow in the same location and direction along the string.

 

[kevklem]

One other thing, when you use two strings a Tolerance parameter is available, Set this to 0 for keeping sharp corners of the section strings throughout the sweep.

 

[hudson888]

http://download.yousendit.com/45F185D7247B0010

Follow the link above to yousendit.com and download the file containing a series of images showing the creation of the helix and groove.

Yousendit is free but only saves data for seven days, users other than Jason who want to follow up after that date may wish to contact me using hudson888@hotmail.com

By the way solutions other than my own may still work. I didn't mention that for the tapered helix creation you need to pick use law for the radius followed by linear, then type in the radii. No curve project at all in required.

In my example I offset some faces to have the groove lead in and out of the bore nicely, but you could extend the curve, prior to sweeping, to make the groove construct slightly longer. It will still work.

Regards

Hudson

 

[hudson888]

Jason,

Thanks for your e-mail after sending you a part with my solution modeled. I thicken a sheet to create the groove. I then also realized that a law extension sheet gives the same result using the tapered helix as the input curve, the tapered bore as the face, and general method, extend both sides, length 0.5mm, angle 90 degrees.

Good Luck

Hudson.

 

[hudson888]

I've been in and out over the weekend checking my computer and occasionally answering here. As per normal I barely finished my previous answer when I realized that the case in fact may be so much simpler that I thought. Jason had shared some info about his part via e-mail, so I know that the groove is 0.4 wide and 0.2 deep with an 0.2 radius, (Jason correct me if I'm wrong). If I'm correct then this is the simplest possible oil groove, and the answer is to create a cable feature 0.4 diameter cable and subtract that from the main solid with the bore in it, using the tapered helix as the centerline.

Good Luck

Hudson