Friday Spiral stumper

[JeffS.]

OK group,

I have a model that is giving me fits. I want to make a plate with a
spiral cut. I have attached a jpeg example. The spiral cut uses a sweep
with a sketched datum created by equation.





Here is the curve equation:
r=.01+t*(.65-.01)
theta=t*360*33
z=.0505

The plate is 0.04 thick and 0.84 by 0.99 with 2 x 0.125 dia holes.

As soon as the cut intersects open features it begins to fail. Anyone
have any ideas?

I am on WF2 , but am open to solutions with WF4 as well.

I can send a part file if anyone is interested.

Regards,
Jeff

Jeff Schnellinger
Senior Mechanical Engineer
jeff.schnellinger@kistler.com
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[TimothyField]

Can you reorder the spiral cut before the .125 diameter holes?


Timothy

[brianlynn]

Might have to make the part bigger to accommodate the entire spiral and
then cut off the excess.

Seems like a bad idea, but I have seen worse situations when I have opened
other individuals parts.

Brian S. Lynn
Technical Coordinator, Product Engineering

[TimothyField]

Looking into it a little bit, It seem to be an accuracy issue. The tighter the accuracy the more "grooves" I could see.

Timothy

[gchampoux]

Create the spiral as a surface/quilt. Then solidify the quilt as a cut.

[JeffS.]

Group,

Thanks for the many helpful replies. I got many suggestions to re-order
the holes, but unfortunately, this does not change the issue.

Here are some more observations:

As long as the spiral is fully inside the part and not intersecting a
hole, it works fine. However, adding a cut to remove excess material
always fails.

As long as a hole is smaller than three individual 'spirals', it passes
through the holes just fine.

So it seems as the spiral has difficulty when encountering many
intersections.

I also dialed accuracy to the minimum I could ( 0.00001) and it made no
difference

I also got many replies to make a surface and then solidify to make the
cut. I have not tried that, but will give it a go.

Thanks for all the speedy help.

Regards,
Jeff

Jeff Schnellinger
Senior Mechanical Engineer
jeff.schnellinger@kistler.com

[ptc-726111]

Hi Jeff,

I also recently noticed a similar problem in SolidWorks when creating a helical sweep cut in a cylindrical part. I needed to cut some flats along the top & bottom of a cylinder where the spiral cut represented the screw threads, and the flat removes the threads in that area. The spiral cut was failing when it intersected the cut-out for the flats. Reordering the features allowed the helical sweep cut to work, but the cut-out for the flat itself failed after the features were re-ordered.

So from reading your message, I suspect this problem is common along multiple CAD platforms (at least for Pro-E & SW), and is not limited to Pro-E. If I can find a method to solve this problem with the part model in SW, I would think a similar technique should also work in Pro-E as well.

Regards,

Chris Thompson

www.appianwaytech.com

In Reply to Jeff Schnellinger:

Group,

Thanks for the many helpful replies. I got many suggestions to re-order
the holes, but unfortunately, this does not change the issue.

Here are some more observations:

As long as the spiral is fully inside the part and not intersecting a
hole, it works fine. However, adding a cut to remove excess material
always fails.

As long as a hole is smaller than three individual 'spirals', it passes
through the holes just fine.

So it seems as the spiral has difficulty when encountering many
intersections.

I also dialed accuracy to the minimum I could ( 0.00001) and it made no
difference

I also got many replies to make a surface and then solidify to make the
cut. I have not tried that, but will give it a go.

Thanks for all the speedy help.

Regards,
Jeff

Jeff Schnellinger
Senior Mechanical Engineer
jeff.schnellinger@kistler.com

[ptc-726111]

Using Gerry's advice, I believe I found a solution and the solution is similar for both Pro-E & SolidWorks when creating a spiral / helical cut. From the attached JPEG files, I created an external sketch (before the spiral cut) of the excess material to be cut-away, and then created an extruded surface after the spiral / helical cut. To cut-away the excess material, select the cutting surface and "Solidify" (Edit --> Solidify). Be sure to select the remove material option and direction in the solidify feature.

In SolidWorks, it is basically the same produce except that you use "Cut with Surface" in-place of "Solidify" (Pro-E). Also, when working with surfaces, let the surface extend beyond the edge of the solid part in-order to successfully cut-away the excess material. The attached images should be sufficient to guide you through the process.

Regards,

Chris Thompson

www.appianwaytech.com

In Reply to Gerry Champoux:

Create the spiral as a surface/quilt. Then solidify the quilt as a cut.