Patterns
Patterns
(OP)
I am trying to create a radial pattern to form five spokes in a wheel. When I use (2) as the number of instances it works well but if I try to change it to (5) it fails. Am I having a problem with this build of Wildfire 2.0.
I'm sure the section I am trying to cut will fit in a 72 degree segment.
I'm sure the section I am trying to cut will fit in a 72 degree segment.





RE: Patterns
Sometimes I have more luck by defining the geometry as surfaces first, making a surface copy of the spoke geometry in its entirety(i.e. the master merge), and then applying an axis pattern to the copied quilt. Then, solidify the pattern leader and reference pattern the solidify feature. So, regardless of how I modeled the first feature, I can always pattern it.
Sounds like in your case, it is referencing some plane which makes everything go nuts when the angle exceeds 180 degrees. I was also working on a spoke design using ISDX (pet project-lowrider bicycle of my dreams
RE: Patterns
RE: Patterns
RE: Patterns
So are they not calling it Surface Transforms in WF? or is it just a circular pattern like SWx?
Best Regards,
Heckler
Sr. Mechanical Engineer
SW2005 SP 3.1 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
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"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux
RE: Patterns
You can still create a surface transform by selecting the quilt, hitting "Copy", then "Paste Special" and applying a Rotation.
It looks like the axis pattern is just an extension of this capability, with some worked in relations to allow you to define the absolute number of copies. Actually if you do what I said above, but set the initial surface copy's rotation to zero, you can then pattern using this zero dimension, and the number of instances can be the total number desired. You would then have to hide the initial quilt which was copied.
RE: Patterns
Steve
http://www.sprdesign.com
http://www.3dlogix.com
RE: Patterns
RE: Patterns
RE: Patterns
It's not that Pro/E has lost functionality. You can do anything in the most recent release than you could have before. If the initial feature is modeled correctly, it can be patterned just as it was in any previous release.
What may be happening is your initial cut is referencing some geometry that is no longer valid once the angle of the cut goes past 180 degrees. It can be referencing a revolved surface using an (offset) edge, which becomes a different surface once it passes 180 (remember, a cylinder technically has 2 surfaces). If this is the case, lose that reference and create a construction circle concentric to the original, and use this for the sketch.
You may also be referencing a Datum plane that causes the dimension to "flip" past 180. If you have created an datum plane at an initial angle for the sketch orientation reference, make sure that the sketch itself does not reference ANY of the default planes. It should only reference geometry that is valid through a full 360 degree rotation (the angled plane, the central axis, and maybe a copied quilt of the inside of the rim).
RE: Patterns
I'm sure if I was willing to work hard enough I could find some work-around to compensate for the loss of functionality but it seems to me as though I shouldn't have to.
I have over 24,000 hours of Pro/E expreience. Based on my expreience with Wildfire 2.0, I can understand why, as I was able to see at the last Design Engineering Show in Chicago, people are flocking to SolidWorks and UG. Wildfire 2.0 is a disaster.
RE: Patterns
But on radial patterns that don't quite
Will generally work. One of the few PTC classes I did manage to get ... and ran into the same problem, not patterning the way it should.... that was the instructors solution...just one of those ever increasing list of work-arounds
RE: Patterns
I never realized that Release 6 of Pro/E came out 2 years before the introduction of the product at Autofact in 1989.
"1989 Parametric Technology ships the first version of Pro/ENGINEER." from http://mbinfo.mbdesign.net/CAD1980.htm
"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.
Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand
RE: Patterns
Can a pattern be mirrored?
I've had trouble with mirroring some clips that have been patterend 6 times. I now need to mirror them across the centerline, and have not had any luck.
The mirror option is grayed out when I select the pattern feature.
Is there a work-around?
David
RE: Patterns
You can create an "old-style" mirror by going to:
Edit-->Feature Operations-->Copy-->Mirror-->(Dependent)-->Done
Select the pattern(s) to mirror, then press Done, then select the mirror plane, and press Done again. (Or just mid click)
This is how mirroring worked Pre-WF, and works in the odd situation when the Edit->Mirror tool doesn't. I am not fully sure why, or what the difference between the two is. All I know is that it gets me out of a pinch.
RE: Patterns
My guess is that the formal roll-out came when they took the product marketing rights, as well as training, back from Autotrol and began their own sales and marketing.
RE: Patterns
RE: Patterns
David