solid part to sheetmetal

[ptc-5799946]

Is it possible to change a solid part into sheetmetal, without loosig any face?

[JamesBurcham]

You can certainly convert a solid part to a sheetmetal part. Its very easy, under options is a button "convert to sheetmetal". How well it will convert is dependent on the solid part. If the solid part is a complex shape that really couldn't or at least shouldn't be made of sheetmetal it may not convert well. If the solid is something that would make sense as sheetmetal the conversion shoudl be simple. I know at a company I worked for converting solid parts to sheetmetal was common practice.

[ptc-5799946]

Yes that is correct, I also often use that. But when we need to change a solid to sheetmetal we need to select a face from the part and that face will be removed.. how to avoid that, if ineed all faces??

[Patriot_1776]

I totally avoid using sheetmetal for anything other than parts that just have simple bends and features. I tried using sheetmetal for stamped parts, that had unique features, and it was a miserable experience.

[ptc-5008082]

In WF5 with your solid model - Applications > Sheetmetal > Shell, do not select any faces and then Done Refs, you will be prompted for the sheet thickness > type in value and <ENTER>

In Creo2 Operations > Convert to Sheetmetal > enter your wall thickness and 'tick' / middle button

you should now have a hollow sheetmetal closed object, you'll need to add rips and bends as appropriate to flatten it.

[Mahesh_Sharma · Accepted solution]

Hi Danty,

If the part which you are converting is of uniform thickness, you need not to shell. You can convert to sheetmetal by defining driving surface. Open Part > Operations > Convert to Sheetmetal > Driving surface > Select any face to define Driving surface for sheetmetal part > Ok. If the part is not of uniform thickness, Creo will report error "The part you are trying to convert to sheet metal does not have a uniform thickness.........".

I hope this will help you.

Regards,

Mahesh

[TomD.inPDX]

Mahesh, I did see a very useful video tutorial to this effect from PTC at one time. Is this available to everyone?

In general, this functionality sounds nice and some have had great luck with it, others, not so much. I have a very hard time using this feature in sheetmetal. I find it faster to define the part in the module from scratch.

[TomD.inPDX]

This is a very basic part that shows the features used to make it.

[bp]

when you are having trouble converting to sheetmetal, most likely your design has some geometry problems. It would be nice if Creo would give some more hints how to fix them but you'll learn by experience..

lately I try to postpone converting to sheetmetal as long as possible, because once you convert, theres no going back without losing every feature you've added in sheetmetal. Sometimes you want to go back to normal mode because sheetmetal mode is very limited when you want to add more advanced features. I even avoid starting in sheetmetal mode because if you change your mind about the manufacturing method there is nothing to go back to.

[Scott67]

Sorry to jump in here but I have a part that I design in wood.  Geometry is simple, it is flat with zero bends.  I am wanting to put a bend in to assimilate a bend like in sheetmetal.  Without adding a bend, the Operation/Convert to Sheetmetal does not seem to work unless I have already put a bend in the part.  Is this correct?

[StephenW]

Convert to sheetmetal will work without a bend but your part will need to be constant thickness BEFORE converting to sheetmetal.

You can do "bends" using warp under the model tab, then Editing drop down in the ribbon.

[Scott67]

The flat part I have, I tried the "Convert to Sheetmetal" but it would not give me the Green Check Mark.  It asked for the Driven Surface so I selected one surface.  Do you have to select all surfaces because it is flat?  I am using Creo 4.0.  Our company is always two to three versions behind.

The wrap feature, I have never seen before.  Actually, there is a lot I have not seen before.  Our company does 99% of there work in sheetmetal so we usually just use the sheetmetal application.  I am sort of venturing  into the unknown during lunch breaks.  The warp feature asked for a direction, how do you tell it a direct without an arrow?  Do PTC Tutorial have something about this?

PTC has some much stuff you can do but it is never in any of their training tutorials in PTC University.

-Scott

[StephenW]

I meant to say spinal bend instead of warp (warp is a little freaky, it'll probably do it but...).

Spinal bend is under the Model tab, Engineering drop down arrow.

For spinal bend, If you sketch a curve, you can make you solid follow that curve.

There are sseveral youtube tutorials https://www.youtube.com/watch?v=kv4qWFel8hQ