Problem with circular pattern

[dixib]

Hi

I'm trying to make a circular pattern, but keep getting the message: "Rebuild error: Only merging features may be patterned. If appropriate, make a pattern of bodies instead."

Do I need to model my part differently to be able to pattern my features?

Hope someone can help with this problem. It's hard to explain, but I think it's obvious what I'm trying to do, if you look at the attached file.

Thanks in advance
dixib

 

[steinmini]

I think you should either create a circular pattern (on a sketch level) before the extrude boss/cut/loft features or try using adding reference plane(s) to do a mirror if that suits your design intention. I'm just a bit confused why not use sheet metal tools to get what you want? A forming tool would do that. And you can re-use it anytime later.

http://www.storyofstuff.org/

 

[dixib]

I've never worked with the sheet metal tools, so I don't know how to use them. Maybe I just need to find some tutorials and get into it...?

I've tried mirroring the features too, but get the same error message.

The part is not a production part, but just a modelling exercise I've given myself (I'm studing to be a technical assistant), so was considering to make sheet metal version later, but right now I just need a model as a part for a computer case (the cover is part of the PSU).

If anybody has some links for good sheet metal tutorials, you're more than welcome to post them

Thanks

 

[steinmini]

I tried to get back to the sketch level of the feature and the circular pattern works fine. Since you've created it, you know what you did, go back and edit each and every feature sketch, use circular pattern in sketch edit mode, and then to the next step... Until you get it done. It appears that your file is older than SW2010 so I can only send you back a parasolid or step file, but I think that you'll enjoy getting the task done yourself. HTH.

http://www.storyofstuff.org/

 

[dixib]

Thank you very much for looking at it.

I'd prefer if was able to do my pattern outside the sketch, since I feel it gives a better structure of the file and simplifies the sketches for later editing.

Yes, it's a 2009 file. And you're right, I'd enjoy it much more, if I make it myself

Think I just have to look into another way of getting it done (maybe with sheet metal?).

 

[steinmini]

Sheet metal allows many things to be done in a single step with some preparation. You have an extrusion, cut and loft and that's three moves. With a well made form tool, that's only one step plus the pattern you need to do anyway. Good luck.

http://www.storyofstuff.org/

 

[JMarv]

The issue seems to be caused by the fact that Extrude10 temporarily creates a separate body. You can't pattern both features and bodies at the same time, but you can pattern them separately.

Here's what you can do: roll back the model and insert a circular patter after Extrude12. (The only thing you need to pattern here is the Extrude12 feature). Edit Loft1 and Loft2 so that they only merge with the raised mount and not the base. After Extrude13, insert a circular pattern to pattern the body. Before Fillet4, add a combine feature to merge the mounts with the base. You will then need to edit Fillet4; and either pattern it, or manually add it to the rest of the mounting tabs.

Joe
SW Premium 2011 SP5.0
Dell T3500 Xeon W3505 2.4Ghz
6.0GB Win7 Pro x64
ATI FirePro V5800

 

[dixib]

Haven't heard the term body in SW before. I'm used to working with bodies in Catia (and miss the boolean features in SW).
Do you know af any ressource to explain the body system in SW, since I don't quite understand why some things are suddenly considered bodies?

The way you propose to do things still seems very complex to me, and not very friendly for later editing. I still thing, that I need to find another way of doing things, to make the file easier to access at a later date (or for someone else).

 

[steinmini]

If you start the wrong way, it is unfriendly to get back and repair. That is why checking out a few video tutorials for the type of work you want to do is always useful. In SW, term "body" is used to describe a 3D solid unlike 2D drawing which has no body. I found that term to be highly intuitive and user friendly since I'm not using English as mother tongue.

http://www.storyofstuff.org/

 

[CorBlimeyLimey]

Multibody Parts;

http://help.solidworks.com/2012/Eng....html?id=6b59fb791b5f421db9dad39acc7a3998#Pg0

Multibody Sheet metal Parts;

http://help.solidworks.com/2012/Eng...s.htm?id=0617ad2177b9437394b9cdca60e0ad3a#Pg0

 

[CorBlimeyLimey]

Here's a simpler alternative.

 

[steinmini]

dixib is using an older version of SW, so am I, and the file is useless from that perspective

http://www.storyofstuff.org/

 

[AnnaWood]

Here is a link to Forming Tools in the SolidWOrks Help files.

http://help.solidworks.com/Search.aspx?query=forming tools&version=2012&lang=English&prod=SolidWorks

Anna Wood
SW2011 SP4, Windows 7 x64

http://www.renderbay.com

http://www.solidmuse.com

http://www.phxswug.com

 

[Updraft]

dixib,

It is evident you are new to SWX. I heartily suggest you go through all of the SWX tutorials. They are excellent! Even if you are experienced with a different 3D system these tutorials will show what SWX can do and how to do them. Your question on bodies will be explained. You will also see and understand why you are having a problem with this patterning.

Do the tuts. You won't regret it.

- - -Updraft

 

[CorBlimeyLimey]

Try this;

 

[dixib]

Thanks for all the links and suggestions. I'll look into it as soon as I get the time for it.