CAD Forum

The more I use Solidworks the more I wonder why we left Solid Edge.

I used to modify the flange profile in Solid Edge. Fairly often. It seldom gave me problems. I did same thing in solidworks then went back and edited the base tab and the flange feature needed the edge redefined. Redefined the edge and bam, the flange profile is back to default and the sketch I had is gone! WTH SW!?!?

Is this what others have experienced? Is the solution to never edit the flange profile? That means extra tab and normal cut features.

Do you have an example of the edits? I've never experienced that.

Edge flanges are finicky in SWX. (Actually, I'm trying to think of something that's not finicky in SWX........ Okay, let's just say that edge flanges are extra finicky. )

It boils down to this: if the sketch line that the edge flange is based on changes IDs or goes AWOL, you can kiss your edge flange goodbye....... and everything dependent on it. And sketch entities can change IDs faster than a politician can switch sides. In your case, where stability is extremely crucial, I would take the time to make separate cuts and not rely on the flange profile.

I occasionally get frustrated at SE's inflexible and clunky UI, but half a day back on SWX cures that pretty quickly.

What would I have to do to break this? I've never had it happen that I can recall but then again, our parts would never change that drastically. If it did it would be a new part number.

jcapriotti wrote: ↑Fri Nov 05, 2021 4:27 pm What would I have to do to break this? I've never had it happen that I can recall but then again, our parts would never change that drastically. If it did it would be a new part number.

image.png

In the sketch of the base tab, if I change the line segment that defines the edge that the flange is attached to the flange feature fails after exiting the sketch. That's no biggie, just update the flange feature to the new edge and accept. The flange should rebuild and all good. Not the case with SW, the profile is gone and the flange defaults back to a rectangle.

Using SW 2019

I have not tested on a flange attached to an edge not defined by sketch, ie. base flange or swept flange. Going to try that now.

edit, added gif of a simplified process. Typically, there's more involved in the tab sketch that causes the flange to fail. But it shouldn't regen the flange from scratch, just update the edge it's on.

@bnemec I see now, it resets the flange when reselect the edge. Same thing happens if you simply edit the edge flange and unselect the edge, then reselect it. I've never done that before, or if I did, it wasn't a custom flange shape.

jcapriotti wrote: ↑Fri Nov 05, 2021 5:49 pm @bnemec I see now, it resets the flange when reselect the edge. Same thing happens if you simply edit the edge flange and unselect the edge, then reselect it. I've never done that before, or if I did, it wasn't a custom flange
shape.

another mine marked

bnemec wrote: ↑Fri Nov 05, 2021 6:04 pm another mine marked
image.png

jcapriotti wrote: ↑Fri Nov 05, 2021 5:49 pm @bnemec I see now, it resets the flange when reselect the edge. Same thing happens if you simply edit the edge flange and unselect the edge, then reselect it. I've never done that before, or if I did, it wasn't a custom flange shape.

I like to get my threads marked as solved if there is some resolution. It sounds like this custom profile being deleted under certain events is not unique to my installation, settings or practice. So, this would be called "Expected Behavior" though undesirable. But once I know I cannot do this I will be more careful.
Thank you.

My sheet modeling in SW so far:

I guess no more editing flange profile. Instead flange, add material with tab(s) then add more cut(s).
I thought I was done with a part but the compare wouldn't come out. The end of a flange was always off, but the sketch was right on the imported geometry when normal view selected while editing sketch. Turns out if the flange angle is not 90 deg the flange produced does not match the sketch. I don't understand what it's doing but I'm convinced that editing flange profile is not production ready. Or am I just doing it wrong, again/still?

Your video looks does not look right. When I edit a flange sketch, the 3D bend shape disappears and the picture returns to the original edge (see image).
I can edit this sketch as often and as radically as I want. Do not, however, replace or move the line in the sketch that represents the edge you selected to make the flange. You can move the ends of that line, but not the line itself.

Dwight

Dwight wrote: ↑Tue Nov 16, 2021 5:36 pm Your video looks does not look right. When I edit a flange sketch, the 3D bend shape disappears and the picture returns to the original edge (see image).

image.png

I can edit this sketch as often and as radically as I want. Do not, however, replace or move the line in the sketch that represents the edge you selected to make the flange. You can move the ends of that line, but not the line itself.

Dwight

HI Dwight the video from Nov 5th shows pretty much what you mention. I wasn't used to that behavior so I lost my flange profile a couple of times. I'm used to the custom flange profile staying even if the edge in the tab sketch is changed.

The video from Nov 15th is showing something else where the flange doesn't match the custom profile when the flange angle is not 90 deg. Maybe I should have started a new thread for that. Another behavior I had not dealt with before but related to the custom flange profile concept. I'm not new to modeling sheet metal, but new to Solidworks. Trying to learn what everyone else has accepted as "expected behavior" vs what I'm just doing wrong in SW.

I looked at it more. I am using SW2018, so maybe they just changed how it looks in your version. Shouldn't make a difference.

I would say that the shift of position you see is due to the shift in the baseline of the sketch. Your bend changes aren't rotating around your sketch reference. You appear to want to position the sketch relative to the axis of the bend, so it does not move as you rotate it. That could be useful, but I don't know if you can do that in SolidWorks. Could you in Solid Edge?

If I needed to do that, I would make an oversize flange then trim it, using a sketch dimensioned to the bend centerline.

Dwight wrote: ↑Tue Nov 16, 2021 5:56 pm I looked at it more. I am using SW2018, so maybe they just changed how it looks in your version. Shouldn't make a difference.

I would say that the shift of position you see is due to the shift in the baseline of the sketch. Your bend changes aren't rotating around your sketch reference. You appear to want to position the sketch relative to the axis of the bend, so it does not move as you rotate it. That could be useful, but I don't know if you can do that in SolidWorks. Could you in Solid Edge?

If I needed to do that, I would make an oversize flange then trim it, using a sketch dimensioned to the bend centerline.

I fear you are talking a bit over my head with positioning the sketch relative to the axis of the bend. Simple terms, I'm expecting the flange geometry to match the sketch I made regardless of the flange angle or bend location/offset or material thickness or bend radius etc.

Here's a gif of SE custom flange sketch at various flange angles, the flange matches the sketch. I didn't bother constraining the sketch, maybe I should have but the point is the flange matches the sketch. In SW the flange only matches the sketch if the flange angle is 90 deg. Or am I missing a setting somewhere?

It only affects modified flanges sketches that are not 90°.

Normal flanges have this option to control flange length. Normally for a non-90° flange it would be tangent to the bend (3rd option.
The problem is when you modify the flange sketch, you lose the option to control flange length. Instead you have to define it in the sketch and you can't easily get the bend tangent point because it doesn't yet exist when modifying the sketch. So for a normal flange, SW is disregarding the sketch length and adjusting flange length based on flange position option selected. You only notice it on non-90° bends. The modified flange on the right I made 2.000 in the sketch but really I want the bend tangent point. Even in SE I didn't see how to get that dimension, although it seems to handle the sketch offset better.