Patterns

[brakemeister]

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.

 

[Guest0527211403]

Have you used an axis pattern or a pattern based on an angular dimension?

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) and the only way I could make my spokes work for me was to do what I said above, since the Style feature referenced my planes for normals and such...

 

[Heckler]

How about Surface Transforms?

 

[Guest0527211403]

The method above using the axis pattern in WF2 has the exact same effect as transforming the surface by 360/N (# instances), then patterning by the same increment N-1 times. That's how I would go about doing that if I was using pre-WF2...

 

[Heckler]

Mark,

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
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[Guest0527211403]

Well.. yes and no.

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.

 

[3dlogix]

Make sure not to set the Angular Offset Datum at Zero Degrees. Pick the default 45 degrees. This usually fixes the problem with not being able to pattern more than half way around a circle.

Steve

http://www.sprdesign.com

http://www.3dlogix.com

 

[brakemeister]

Thanks for all your posts but, I guess, the bottom line is that Pro can't do what it used to do before with ease. I've gone ahead and done it as (5) seperate cuts. Hopefully they will be able to get this thing fixed.

 

[stephenweinstein]

This is not the "correct" answer, but I often "cheat" in this situation by repeated mirroring about datum planes that I create 1/2 way between the existing feature and the one that I want to add.

 

[Guest0527211403]

brakemeister

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).

 

[brakemeister]

I have been successfully creating patterns as well as reference patterns since Release 6 in about 1987. I have never had a problem such as this. In 1992 I began design of the Harley-Davidson VR1000 Race Bike Chassis using Pro. It was introduced in Feb 1994 at the Daytona 200 mile race. Used lots of patterns in that design. Worked fine.

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.

 

[cadcamguy]

Can't tell you about WF , seems the more I hear about it the more I want to stay with r2001

But on radial patterns that don't quite pattern correctly.. do a copy rotate , then pattern that.
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

 

[looslib]

brakemeister,

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

 

[davidinindy]

Speaking of 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

 

[Guest0527211403]

Sometimes the mirror tool doesn't like my patterns either.

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.

 

[brakemeister]

Pro/E was origionally sold solely by Autotrol Technologies in Thornton, CO. At that time, while it was called Pro/ENGINEER, it was marketed as an Autotrol product and, since Parametric Technology had no interest in making drawings with Pro, it was marketed with Autotrol Series 7000 with Pro as the solid modeler and Autotrol as the drafting package.

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.

 

[stephenweinstein]

Even if mirroring features does not work, mirroring the entire part may work. Depending on which release you have, this is either Feature > Mirror Geom (which is the entire part; to mirror individual features was part of Feature > Copy) or "Select the Part name in the Model Tree > Edit > Mirror".

 

[davidinindy]

Well, mirroring the whole part worked on my dummy part, but won't work in the situation in my real part. I don't have time right now, but I think mirroring the part, then patterning the original and the mirrored part might work.

David