CAD Forum

I'll start by saying, I don't do a lot of sheet metal....
When inserting an edge flange feature I notice that you get the option for flange length (Blind and up to vertex).
When you select Blind and give it a dimension, it creates the sketch and feature but the sketch comes through as under constrained.
This dimension can be modified in the FEATURE but the sketch remans under constrained.
If you modify the sketch and add a dimension the sketch then becomes fully defined and the feature BLIND dimension disappears.

This does make sense to me BUT why does the sketch not generate as full defined when you 1st make the feature?
Is this something that I have to get used to or is there a reason?

Further more, if you go back to the sketch and delete the sketch dimension the Blind distance option comes back.
I understand but WHY.

I don't think there's a reason but I've always pondered the same, why isn't the dimension in the sketch to drive the feature, rather then in the feature to drive the sketch.

Bryan O wrote: ↑Wed Oct 04, 2023 4:43 pm Is this something that I have to get used to or is there a reason?

Get used to it, a few features do same thing.
Famous one is pattern.

It's been like that f..o..r..e..v..e..r. I wish that if you typed that in, you could chose ID or OD and then it would dimension the sketch appropriately.

For simple parts with an edge flange it's kind of annoying, but if you do enough complicated parts where you have to go in and edit the flange anyways, it's kind of nice that is does it that way so you don't have to remove it. Kind of like glass half full or half empty, all depends on your perspective and what your doing.

Actually I'm to the point now that I just drag it after selecting the edge and just drop it anywhere in the direction I want and don't even bother putting in a value anymore, then I just edit the sketch and define it there. The workflow becomes intuitive once you start using it often.

Bryan O wrote: ↑Wed Oct 04, 2023 4:43 pm This does make sense to me BUT why does the sketch not generate as full defined when you 1st make the feature?
Is this something that I have to get used to or is there a reason?

Its the way they implemented to give flexibility in modifying the underlying sketch. The OCD in me doesn't like that it shows the sketch under defined either. They should've overridden the system check on those unless you modify it.

Whether they show the "Length" in the flange property manager is based on the far side sketch line and if its parallel to the edge. As soon as you remove the vertical/horizontal relation and make it no longer parallel, it disappears. You can mess with the sides all you want.
I think this has to do with how they control the flange length as you have 3 options: Seems they internally move that far side parallel line based on the length value and those options. For 90° it's easy, just inside and outside faces. For non 90° bends its having to calculate the virtual intersections for the first two options, and the tangent condition which now drags the radius and thickness into it. Adding a sketch dimension length to handle these is near impossible.

Bryan O wrote: ↑Wed Oct 04, 2023 4:43 pm
This does make sense to me BUT why does the sketch not generate as full defined when you 1st make the feature?
Is this something that I have to get used to or is there a reason?

I don't know why & I have come to the conclusion that I'm not sure that it matters. It is the same question asked in the past by others and has people on both sides of the fence, "Do I need all my sketches fully defined or not?"

When I started working with 3CAD (SolidWorks) 2 years I ago I had very little experience in CAD of any sort & only entered dimensions & constrained the features that I knew the dimensions for. The rest I left as they were. My boss after a week or a few said that I should constrain my drawings so I started using fully define sketch option. But I soon discovered that that wasn't always what I wanted!

TTevolve wrote: ↑Thu Oct 05, 2023 8:29 am Actually I'm to the point now that I just drag it after selecting the edge and just drop it anywhere in the direction I want and don't even bother putting in a value anymore, then I just edit the sketch and define it there. The workflow becomes intuitive once you start using it often.

I follow this work flow quite a bit but in some cases it makes more sense (to me any way) to just use blind & enter in my dimension. In the example below if I would've had to enter the same dimension 4 times for the height of the flange or use a global variable (which I haven't done much of). Either way would be fine. Except that for a simple part on a simple assembly of just a few parts do I need to set up global variables? & to make changes do I want to change one dimension or multiple dimensions? My 2 cents for what it's worth.

For a simple box I wouldn't bother going into the sketches to constrain them fully, if you don't move the sketch lines of the edge flange they stay linked to the flange length valve in the feature creation box, so if you have to modify them all at the same time you can. I rarely do simple edge flanges though. I actually like using miter flange more now then edge flange because you have the option to add additional flanges if you need to.

Now that I get some input, I understand what it does and why it does it.
I was compared it to other features like Hole Wizard which does define the sketch.
I can see how if you wanted it for just square flanges it would drive the OCD/fully dined driven people but I also see the benefits for "custom bend"

Bryan O wrote: ↑Fri Oct 06, 2023 11:07 am Now that I get some input, I understand what it does and why it does it.
I was compared it to other features like Hole Wizard which does define the sketch.
I can see how if you wanted it for just square flanges it would drive the OCD/fully dined driven people but I also see the benefits for "custom bend"

As OCD about these kind of things as I am, I've never gone back in to fully constrain these sketches. I've been making sheet metal parts in SolidWorks since before the edge flange existed. Never been an issue.

Now, if they would just fix the highlighting text when you dynamically drag the edge flange length on creation so you can type the length on the fly....broke in 2019...still broke in 2023.

jcapriotti wrote: ↑Fri Oct 06, 2023 1:39 pm Now, if they would just fix the highlighting text when you dynamically drag the edge flange length on creation so you can type the length on the fly....broke in 2019...still broke in 2023.

Yea, that would be nice!

On the whole constrained vs. unconstrained sketches; if you use the software long enough you will eventually come across a time when you modify something and other holes/edges/cuts/...etc. don't go where you want them because they are unconstrained.

TTevolve wrote: ↑Tue Oct 10, 2023 11:44 am Yea, that would be nice!

On the whole constrained vs. unconstrained sketches; if you use the software long enough you will eventually come across a time when you modify something and other holes/edges/cuts/...etc. don't go where you want them because they are unconstrained.

I fully define all sketches....except for the flange sketch as its has a "soft" fully defined condition with its length parameter. Have never had an issue with it, and we rarely if ever modify the underlying sketch.

I think the assumption is that if you are editing the sketch you are doing something beyond changing the length. Edge flanges feature can contain multiple flanges. Each can be edited to different length or even totally different shape. There is no way all this can be fed back to a single dimension in a dialogue.