how do i make edge flaps on an angled surface?

[srosefx]

hi
im having trouble in putting edge flanges on a surface that is angled but i would like the tabs to be parallel to the surface like in the picture.
thanks
simon

 

[Gupta65]

I tried one simple example and it worked fine. Can you upload your part to review.

Deepak Gupta
SW2009 SP4.1
SW2007 SP5.0
MathCAD 14.0

 

[mjcole]

You could use this method for now I'm pondering others

Michael

 

[Gupta65]

Michael, I have modeled the similar way.

Deepak Gupta
SW2009 SP4.1
SW2007 SP5.0
MathCAD 14.0

 

[srosefx]

hi
wow that solution was fast and seemed to look great, but is it a sheet metal part?

when i make my sheet metal part from my spline, and then i cut a 6.26degree angle off the bottom, it will not let me make tabs and it doesnt let me unfold "has beveled edges cannot flatten"

am i building this wrong?

i am a new user and feel a bit thick

thank you kindly
simon

 

[Gupta65]

Don't use tab but use edge flange tool.

Deepak Gupta
SW2009 SP4.1
SW2007 SP5.0
MathCAD 14.0

 

[srosefx]

i made a spline profile
then i made clicked insert->sheet metal->base flange

hieght of eg: 100mm

then i cut the angle off with a closed spline and extruded cut

then i wont let me flatten or make edge flanges!!!

 

[CorBlimeyLimey]

Sketch33 had an extra line, but after correcting that it worked fine for me with SW2010-SP2.0

FYI, a closed loop is not needed to make a cut. A single line will suffice.

 

[srosefx]

maybe its the version im running 2008 sp0
ill try my update see what happens.

i tried the single line cut worked great.
but when i flatten it wont let me do that either.

cheers

ill try 2010 and see.
simon

 

[mjcole]

I am having difficulties launching 08 but don't want to do a repair because both 2009 and 2010 are working and I'm happy.

I too noticed the extra lines but one was construction and there was a closed region so it worked fine on my 2009 model. I have a friend still running 2008 maybe I can create a wmv with RX for you.

Quick thing to check. Edit the Cut feature and see whether or not the
[]Normal Cut option is checked off it may be causing the Part contains features that cannot be unbent" error.

The technique I used was to create a new sketch and extract the 2 sketches for flange profile from the original flange sketches. because when you delete the old edge flange solidworks demolishes the sketches and doesn't give options to keep them or roll back the flange feature.

With a single sketch created prior to the cut you can dimension both flanges in a single sketch and create an extruded surface to use as a reference for your Flange Profile sketch.

While in sketch mode drag the end points of line on model edge off the extents this will allow you to position the profile based on the extruded surface. This can be done using a pierce point to the edge on surface body or by creating an Intersection curve using the parallel face of the extruded surface while editing profile sketch.

Video of the process described is attached.

Michael

 

[mjcole]

Below

/!\ Please Enter Your Message in the Message Area Before Submitting.


Michael

 

[CorBlimeyLimey]

Michael ...

Why go to all that trouble? Simply invoking the Edge Flange tool, and selecting the two edges involved, automatically recreates new sketches.

 

[mjcole]

My thinking is that with this method you can control multiple flanges in a single sketch instead of the two auto created ones using the selected edges.

The sketch can be edited to control both profile shapes at the same time and auto update. Selecting the edges gives you 2 rectangles.

I wholly agree with you if the flanges are rectangular but if they have more complex profile I think the reference surface is useful. In this case I saw that the flanges that existed were dimensioned to the uncut shape.

Since the sketch plane would be at an angle to the top face it would make the dimensioning harder. If I projected the curves with Convert Entities the position would be normal to and not along direction.

Michael

 

[srosefx]

thank you all for the result,
i tried it last night and it was just the normals setting i failed to try.

it worked great and my model is now complete.

i owe you all a beer sometime.

simon