Ellipse sketch pattern

[ctopher]

I noticed recently in SW 2011 when I create an ellipse, then do a linear sketch pattern, the ellipses are no longer associated dimensionally. If I change the first ellipse, the others do not change.
But, it works with all other shapes.
Has anyone seen this? I can create the sketch with arcs, but it's interesting that an ellipse will not work.

Thanks

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[mjcole]

Chris,

Interesting Catch, May be a bug but try the following workaround. I'll try it on 2010 and see if I get the same behavior. My old machine that has SolidWorks doesn't support 2011 boo SolidWorks 2011. I don't think I ever really patterned ellipsi Sketchwise.

You may want to try the Equal Ellipse Relation.

CTRL Select 2 ellipses or drag a Right To Left Crossing Rectangle and Select equal Constraint from the pop-up constraints menu.

Strike That the Equal Relation I was thinking of is for Equal Slots which is an option but not so for Ellipses.

You'll have to do SolidWorks job for it the Pattern Relation doesn't even keep the centers aligned to the pattern grid after patterning. This cannot be anything other than a bug. Or an extreme oversight by Product Definition and the Development teams. Maybe an Enhancement request is in order that says sketch patters should work properly. Development will probably tell you that Sketch patterns weren't intended for anything other than Lines and Arcs. Or that you should be using a Feature Pattern. But this is indeed a bug.

This flaw goes back to 2009 version which I just tested. Maybe an Equal Ellipse relation could be added in to solve this issue. It's great for Slots but why should they have all the fun?

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[ctopher]

Michael,
Thanks. The Equal Ellipse relation works.
Yes it's weird the linear pattern doesn't work.
I'll send it in as a bug.
Curious if anyone sees it on SW 2012?

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[ctopher]

UGH!
I meant equal "slots" relation works.
Yes, it should work for ellipse also.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[mjcole]

I forget if I tested this on 2013 Alpha I saw a few long broken issues in SolidWorks all of a sudden worked correctly in 2013. But it surprises me that I didn't find this bug. I guess I assumed the Pattern function should work without issue now that they added Dims for pattern parameters and other things.

It should all work but Software Development is hard and for the most Part the SolidWorks team does pretty well at it.

Please post the SPR number if they make it a bug report.

Thanks,

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[ctopher]

Thanks. I just turned it in.
ER # 1-3012307572

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[mjcole]

Chris,

Thanks for the reporting and telling us the ER info. SPR would indicate bugfix which they may also do if the patterns were originally supposed to work for non Line Circle Arc figures. But until then, to have equal ellipses would be cool and work for non pattern cases. it is also probably easier to achieve.

Another Workaround has a little more set up but should work better.

The third 3rd method would be to use a block which I'll try next. But my current and tested method is too Pattern two perpendicular lines with a set of (midpoint, coincident, intersect) to get a set of

_|_

Perpendicular lines and a crosspoint Pattern these 4 items (2 lines) 1 centerpoint (1 point) on (1 Ellipse) concentric (o+)

I suggest making the lines not exactly on quadrants of ellipse since those will not be maintained by the pattern. After the pattern operation you can add however many Xdir Ydir instances to place the quadrant points on the patterned lines which maintain the size and shape of the ellipse.

I will post a 2009 set up part with three sketches with 1 method each. Dimensions Before Dimensions After Block in Sketch for everyone to test out in various versions of SolidWorks you may even use it to attach to the ER as a test part for the developer teams.
Other methods of maintaining the pattern can be a set of 2 centerlines for angle and length dimensions for pattern centerpoint spacing and using Linked Dims and coincident relations between ellipse center and line and 1 quadrant and pattern direction line.

Using a construction Slot and linking in the Quadrant points of the Ellipses with arc and wall centers. You may even get the pattern axes to show at the centers.

Well SolidWorks crashed on last attempt so I'll get the model together tomorrow and post the file here.

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[rstupplebeen]

I use ellipses all the time for optics and they are a temperamental bunch. I have not had the need to pattern however I routinely use intersection curve or convert entities. They appear to work well until the ellipses has the same major and minor diameter effectively creating a circle. Once this happens the intersection curve or the converted entity is now stuck as a a circle even if you change the major and minor diameters. Basically use with care.

As another work around can you pattern the feature that your are creating instead such as a thru hole?

I hope this helps.

Rob Stupplebeen

https://sites.google.com/site/robertkstupplebeen/

 

[ctopher]

Rob,
Yes I can pattern the feature.
I was only bringing up the issue that the ellipse can't be patterned in a sketch.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[mjcole]

Hey guys,

Here is a test model for the Ellipse Pattern and several methods as I've suggested and tried to explain.

Method 1 Pattern (Lines Points Rectangles) that will drive the size and placement of the ellipses.

Method 2 Create a Block (Sketch Group) of your ellipse.
Pattern The Block. If you add dimensions before the Block they will no longer be shown by sketch but can be accessed by editing the block to change Size and Orientation of the ellipse. Using a patterned construction Slot and a non aligned Ellipse you can control Ellipse Radii and orientation by placing 3 midpoint or coincident to side flats end arcs or Centerpoint.

Ellipses get patterned but are not constrained by the Patterned# relations which is shown when relations are shown in sketch. Try doing a pattern of an ellipse and any other entity. Edit that pattern and you'll see the ellipse is not in the entities to pattern Selection Box grouping.

ETqid=331847_EllipsePattern_Fail-CFG

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[mjcole]

Use Link below post the http:// causes problems lets try it again
Partname:ETqid=331847_EllipsePattern_Fail-CFG.SLDPRT

Link pasted Works

http://files.engineering.com/getfil...e=ETqid=331847_EllipsePattern_Fail-CFG.SLDPRT

Link using {Link} {/Link} square braces: Link Shown Below problem
Entered as {TGML} Link{/TGML}



"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks