Hello!
I'm trying to unfold part in attached file. I have seen some tutorials on Youtube on how to do that, but evrytime I try to selct an edge with insert bends I get "Cannot use this kind of edge" tooltip. Sow how can i get a flat version of the part, so i could cut it from wood?
Cheers, Matjaz
How can I make it in sheet metal? Thsi part was created in assembly by using loft feature. But lofted sheet metal supports only 2 profiles and no guide curves...
But you want it flatterned. Once you have a bend in it, Slolidworks needs bend deductions, k factor ect... to arrive at a flat patten.
The thickness has to be contant too.
I only know that sheet metal can do this.
To be able to flatten it, there must be a base flange somewhere.
Think about trying to flatten an egg shell with your hand and trying to get a flat patten.
Not the most elegant solution, I'm sure, but it works. You may need to adjust the bend radius to suit your needs.
Patrick thank you for answer!
Unfortunatly I'm ussing SW 2012, and can't open your part. Is ther any way you could save it as SW 2012 part? If not, can you please explain the adjustmen of bend radius in details (to what value heve You changed it etc..)?
Sorry, I only have SW 2013. Here is a breakdown of what I did though.
1) Delete existing loft (leaving behind sketches)
2) Create a sketch on the front plane
3) Use Convert Entities on two of the lines in 3DSketch1 to create a profile
4) Using the new sketch I created a Base Flange feature with a 3mm thickness and 6mm bend radius
5) End conditions 1 and 2 were set to "Up to Vertex" and I used the endpoints of the lines in 3DSketch1
6) Finally I added cuts to follow the angled edges in 3DSketch1
I've attached a screenshot so you can see the feature tree.
Thankyou, that did the job. But I have probem with cutting those corne off. I see You did it by using surfaces. Di you use 3DSketch1, or did you project that sketch to new plane and then cut?
I created the plane perpendicular to the angled face of the part and coincident to one of the edges in 3DSketch1.
Check this one!
I couldn't get that part to flatten. Did it work for you, or is it just something on my end?
Sorry; RoundBend1 @Convert-Solid1 was suppressed and I corrected it. (I uploaded the correced one.)
If you follow the sketches, interpolation curve (@Sketch2) between two flaps have a twist and therefore it should be considered as forming process.
So what I did is; make two surfaces and get the proper interpolation curve.
Make the part in sheet metal, so much quicker.