Inserting bends on solid body w/ radiuses

[PCS74]

I am having problems.

Is there any way to unfold a solid part with radiused corners or insert bends on radiused corners?

Due to part geometry I cannot create edges, insert bends and then specify the radius.\



Chris S

 

[CorBlimeyLimey]

Sorry, I do not understand the question. Could you post an image of what you are trying to do. See faq559-1100.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[MadMango]

Several things to consider:

equal part thickness of all features
straight bends in the bend region only, nothing curved
no variable radius bends

[green]"I think there is a world market for maybe five computers."[/green]
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Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[PCS74]

CorBlimeyLimey,

Thanks for the info. Pics are located at:

http://img212.imageshack.us/img212/912/funnelpic13eh.jpg

http://img97.imageshack.us/img97/971/funnelpic28qa.jpg

Now,

This is actually two parts and I am not trying to unfold them as is. I am trying to flatten them separately. As you can see there are no selectable edges that I can insert bends on in this model. It was made using a lofted boss and hollowed out using a lofted cut. The radiused edges were incorporated into the sketch as fillets(hence no selectable edges). This is how I need the finished part to look.

I have tried to create this model in two other ways:

First,

Create a lofted boss and shell it. This leaves a selectable inside and outside edge which allows me to insert bends. However, when the desired bend radius is inserted the upper and lower surfaces are deformed. Solidworks tries to make the bend, but it also tries to keep the corners. See pic below

http://img226.imageshack.us/img226/8165/funnel2frontpic5kl.jpg

I have also tried to add radiused edges to the part when created this way, but it creates unusual geometry at the top and bottom corners. See pic below

http://img65.imageshack.us/img65/1053/funnel2pic14oj.jpg

Second,

Create a body via extrusion, extruded cuts and shell feature. It makes the bend and flattens the part, but it adds "cuts" in the base around the bottom of the radius and the tops look like those in the third pic I posted.


Any help is greatly appreciated,

Chris S

 

[CorBlimeyLimey]

1) Eliminate the radiused corners from the sketches in the loft.
2) When using the Insert Bends, just select a flat surface ... SW will find all bends involved & apply the default radius to them.
3) RMB on Flatten-Bends, select Eit Feature & change the default radius.

The Flatten function should now work.

BTW, this is for SW2004. What are you using?


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[CADGemini]

PCS74,

Instead of using solid features to create this part you should be using the sheetmetal features. For this part I would use the lofted bends feature. I was able to flatten the part after using those features.

By the way what version are you using?

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

Solidworks 2006 SP0.0

 

[CorBlimeyLimey]

The Lofted Bend function is definitely the easier way to go, but it will not give accurate bend radii. The radii in the sketches are being extruded/swept/lofted through an angle, so the resultant fillets will not be a true radius.

If you do a lofted Bend you will notice that it adds a radius to the flattened profile, at the bend ends. You can easily reproduce that in the Inserted Bends method to eliminate the peaks shown in your 3rd image. You will also end up with a true radiused fillet.

So, use whichever method works best for you.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091