1-Visitor

Question

Why in creo sketch there are no linear and circular pattern options?

Forum|Forum|9 years ago
January 21, 2017
10 replies
47670 views

Dear Creo users,

While doing some complicated sketch don't you think there is a need of linear and circular pattern options in creo sketch? Its true pattern option is given in solid modelling and we can pattern a feature or group of features. In solid works users can pattern inside sketch mode. in creo 3.0 and 4.0 is there any updates on sketch pattern? I am using creo 2.0.

With regards,

Soumya

General

S

six10

10-Marble

There is no pattern function inside sketcher in Core 3.0. As far as I know, the workaround is to make a sketch, and than pattern the whole sketch. As a previous SolidWorks user, I find this very annoying.

T

TomD.inPDX

17-Peridot

Because Creo is not Solidworks

N

NB_10150484

1-Visitor

Are you proud CREO fails to offer the features?

D

DK_11195542

3-Newcomer

They absolutely are, and its pathetic.

M

MartinHanak

24-Ruby III

Hi,

in Creo 3.0 and 4.0 you also cannot pattern geometry in Sketcher mode.

MH

T

TobiasLarsson

12-Amethyst

when do you want to pattern inside a sketch? Seems like you would create an unnecessary complicated sketch? Please enlighten me!

//Tobias

C

creuz

1-Visitor

What if you just want to draw a daisy?

C

Constantin

15-Moonstone

You draw and extrude one petal and pattern that.

I

iullah

1-Visitor

This is PTC's strategy to keep sketch as simple as possible, so no linear or circular pattern. Also there is no need to do so. I have used CATIA sketcher, NX sketcher and Solidworks as well, but honestly speaking Creo sketcher is the fastest.

If you need to use linear or circular pattern, you probably want to have a 2D sketch, and Creo is not meant for this purpose.

T

TomD.inPDX

17-Peridot

Complex sketches is one of Creo's strong points. And I love them. But Sketch patterns were not a concept for early developers and today, there is no push to add it. This would be a serious re-write. Not to mention that the SW version is far from robust. PTC doesn't do anything unless they have the opportunity to make it 10x what SW would have.

What I really miss is "midplane"... just as a matter of convenience. That may have other implications to incorporate.

S

six10

10-Marble

I am probably not expereinced enough Creo user to give a credible opinion on this, but after more than a year of 10 hours per day in Creo, i still find sketching bad. Offset and project sketch specially. The contour is never ever whole, always space -red dots- between lines. Sometimes even on very simple geometry.

S

sbhattacharya-2

Author

1-Visitor

Hi all , Don't you think that this sketch can be better drawn by using sketch pattern option if it is in Creo sketch?

I have seen an option called copy and paste special in creo sketch. In this option have anyone tried to rotate a copy of sketch at a specified angle?

Thanks for all your replies. Any other suggestions or discussions will be helpful.

Is there any portion in this community or ways to request or connect PTC Developers about some enhancement that creo users like to request?

With regards,

Soumya

K

Kevin

1-Visitor

‌Maybe it's a matter of preference or just the way I learned to use ProE but I wouldn't include all that detail in a single sketch feature. Not that it necessarily is but I think I would find it easier to create the ears and the associated holes as their own features or group of features and pattern that. You also lose the advantages a feature pattern can offer although you do have other options you could use for those.

D

dcaucutt

1-Visitor

As a work-around you could pattern the sketch feature. After that you could create another sketch referencing the patterned sketches.

C

ckeller

1-Visitor

I often use streamlined "skeleton" sketches that I then reference in a final sketch. This allows me to lock down and simplify the most important relations and then the more intricate details of the final sketch are kept separate. as a simple example, you might have a complex polygon that you want to have radii on. it is much easier to sketch the radii-less polygon and then in a subsequent sketch use edge, pick the loop - and add a bunch of fillets to the sketch.

you might think, well why not keep it simple and in one sketch? actually it's not as simple to have in one sketch. if it fails - you can see where it fails. and for my example, the dragging the radius bigger or smaller doesn't affect the shape of the polygon, etc.

when I need a sketch to have a pattern, I often will create the prototype shape, then pattern it, then create the final sketch and just use edge -> loop.

if you don't like to see separate sketches, then group them.

it works, it works well, and it's just the way this software works. I personally wouldn't mind if there was a way to create patterned sketch features within a sketch. however it would just be a novelty to me. after 20+ years using pro|E / Creo, I can confirm - simple sketches are more robust. and more complex sketches are more robust when broken up into multiple steps.

The attached video shows this 2-sketch method. it's for a complex polygon and a simple radius. if you included the radius in the original sketch dragging would be horribly unwieldy. Anyway - the same concept works for patterns.

Video Link : 7509

S

sbhattacharya-2

Author

1-Visitor

Hi all,

So to sum up I conclude that if we pattern in sketch mode

1) Sketch will be unstable and there will be no associativity or connection between sketch pattern members like in feature pattern

2) It will be very difficult to increase the no. of pattern, angle or spacing members after sketch pattern as there are no connection between pattern members.

But for information, I would like to say that in Autocad 2013 to 2017 Autodesk have introduced a property called array associativity. If you select the members after array the array will be selected as a group. You can also explode it and make separate anytime you want. Though I am aware that autocad is primarily a 2d drafting software and nothing comparable to feature-based, parametric 3D CAD software like PTC Creo but if this feature can be applied in creo sketch then one can easily get a feature pattern like sketch-pattern.

What do you think?

I am interested to know what other Creo users think about this.

R

rohit_rajan

15-Moonstone

What about fully defining the complex sketch?How will creo define how to dimension it?

Anyways if you have current maintenance for Creo you can put up this in PRODUCT IDEA.

N

NitMad

10-Marble

You can always copy paste the entities you want and then, select the first one and the copied one copy it again and paste it ad infinitum while changing the offset in the required direction. But, as pointed out in the other answers, it will complicate your sketch.

H

Hbaq121

10-Marble

Sketch needs the ability to create a pattern regardless. Patterns and mirrored are not the best solution, but they need to be available. Sometimes a very good occasion arises. My past experience has showed me that it's better to keep most anything that can be done in a sketch in the sketch form and not patterning features of the extruded.

Patriot_1776

22-Sapphire II

Having transitioned after over 10 years from AutoCAD to Pro/E in '96, I wish the sketcher was better and did have patterns available in sketcher, but, though it's more tedious, you can manually create whatever pattern you need. It's not a huge deal unless you make it one. 😉

Sign up

Please use your PTC eSupport account.

Welcome to the PTC Community

Please use your PTC eSupport account.

Scanning file for viruses.

This file cannot be downloaded