Adding wall at non 90 deg changes size

WF 2.0, not much experience with sheetmetal.

I am modeling a sheetmetal part. I want it to basically look like this:

/__________\

With two flanges or flat walls at 45 degrees from the initial wall.

I start with a 12 x 10 inch unattached flat wall. I then add a flange wall or a flat wall with a bend radius. The problem is, now my part is no longer 12 x 10. Giving the wall an angle of less than 90 degrees (with respect to the initial wall) effectively shrinks my part. I have tried different options and material sides and offsets and whatnot, but have not found a way to do what I want. With no bend radius it is ok. I suppose I could try to fudge it, but I don't want to. What's the point?

I would think the program would have an option to maintain the outline size (design intent) of the original wall or somesing.

Any help?

Edited by: AchrisK

Are you sure you are accounting for the edge bend?



What I do on something like this is dimension it using the intersect
option, picking a side wall and the face and repeat on the other
side. This will ensure that you are dimensioning to the sharp
corners and not the bend itself.



I hope this helps.

Jim

One other note to mention. You should be able to draw the entire
profile as a sketch, then extrude the sketch. The extrude command
will let you add bends to the sharp edges. You may be able to
save yourself time with fewer features, as you could do all three walls
in one feature.



Just a thought.

Jim

Thanks for the reply.

My problem is that I want the physical size of the finished part to be 12 x 10, so I don't want the bends to "subtract" from the finished size of the part. With 90 degree bends you can either have the material thickness within the original wall size, or one material thickness beyond the original wall size. Your choice depends on your design intent; weather the size of your object is more critical, or the space within your object is more critical.

What I think is happening is Pro is taking the above idea, and when a bend is more than 90 degrees (forms an acute angle with the initial wall), instead of maintaining the same center point of the bend, it is allowing the bend to travel toward the middle of the part, effectively shrinking the original intended size.

I assume that if my intent is to have a part at a given size in its bent state, that Pro/E should be able to deliver that. I would be pretty surprised if finished sizes of any non-90 degree bend are just left up to chance (not really chance, but you know...).

Chris

I am attaching a picture of a bend similar to the one you are
doing. Notice the walls are driven from a curve. You can
see that the wall follows the curve, but only leaves the curve at the
bend. This is to allow for the radius of the bend. But the
front and side walls clearly follow the curve. Is this what you
get? If so, then it is coming off of the curve for the
bend. If not, then I am not sure what is happening. Can you
post a similar screenshot?



If the problem is the corner coming off of the bend, you may want to
sketch a curve with radii constrained so you get the final look you
want. Pro/E should interpret the radii as bends and keep the
shape you want.



I hope this helps.

Jim



View attachment 2476

I understand what you're saying. That is the situation that exists in AutoCAD when you draw your shape and then add radii, or even in sketcher; adding radii between two walls that are in a somewhat fixed position. The thing is, in Pro/Sheetmetal, we are supposed to be building a different way. In Pro, we are placing the second wall, radius and all, all at the same time.

I do realize I can probably get my result from sketching out a wall (or thin) profile and extruding it. But then, say I have that type of feature on three or four sides of an initial wall (I have a part with that on three sides). Then I suppose I can do the above for the first wall and two of the sides, and then figure out how to sketch the profile for the third bend/wall. But I want to know if the functionality exists in Pro/E to model this type of thing on purpose, based on design intent.

Here are some screen shots. You can see the original wall in grey and the new geometry in yellow. You can see that the 90 degree bend allows for desing intent, and the 135 degree bend does not.

View attachment 2477

View attachment 2478

View attachment 2479

View attachment 2480

I think I may have figured out your problem. I hope you are using
WF3, as I do not think this is in WF2 (or I do not know where to go if
it is)



Here is the problem you have:



View attachment 2481



Here it is with the "Offset wall with respect...." option checked



View attachment 2482



This appears to achieve what you are trying to do. I think this
is new in WF3 though. It may be possible in WF2, but like I said,
I do not know where the option is.



I hope this helps.



Jim

I am using WF 2.0

That would indeed be the condition I am trying to achieve. But I am pretty sure I have that option, or an option that looks like that. I tried it and it didn't seem to do what I wanted.

Which wall feature did you use? Flat or Flange? Which edge did you select to attach the new wall to, the uppr or lower?

I will go mess with it some more.

Chris

Yeah, this feature seems like it may have been broken in WF 2.0 (M130). when I just select offset and let it default to automatic, nothing changes at all, or it moves one material thickness, depending on how I have the "changes thickness to other side of sketch plane" button set. But neither case brings the outside of the bend tangent with the original edge of the first wall, as it shows in your example.

Also, it will not allow negative values. A neg value just defaults to a positive value, so that any value placed in the box pushes the feature further waway from the attach edge.

Here are some screenshots:

View attachment 2483

View attachment 2484

View attachment 2485

View attachment 2486
Edited by: AchrisK

I didn't use WF2 too much, as we just recently jumped from
ProE2001. WF3 was at build M020, so I figured just go with the
latest.



I created the first wall as a flat wall. I then used the bottom
(of the picture) edge as my attachment edge and used the flange tool
for the side wall. I used a value of 135 degrees for the bend.



If you have maintenance, you can download WF3 and try it. I love it.



If not, you may want to check which build you are using and see f there is an update.



Nevertheless, I would send PTC an email informing them of this problem
in WF2. Especially if you plan on staying with it for a while.



Good luck,

Jim

Jim,

Thanks for your time and help on this. I don't mind working around this issue, knowing that PTC has already addressed it. That is resolution enough for me.

We do have current maintenence, so I'll have to look into when the company plans to go to 3.0. I am pretty new here, so I am not sure what their policy is on that. They don't allow admit rights, or even power user rights on our computers, so I can't do flipping anything without having the IT dept do it for me. Kinda sucks. Not used to that.

Thanks again!

Chris

No problem. Anytime. This is what makes this forum so
great. Everyone helps in any way they can. I have learned
more from this forum than I have at all of the PTC classes I have
attended.



Luckily for me, I am the CAD/CAM Administrator here. I pretty
much get to run the show. I am the only one running WF3, but plan
to implement it company wide once I get a little more familiar with
it. We also only have around 6 seats of Pro/E, so it is pretty
easy to manage.



You may want to try and convince them of the benefits of WF3. We
do 95% sheet metal work, so it is a no brainer if you have used sheet
metal from 2001 and prior. WF2 is much better, though I quickly
switched to WF3 and didn't spend a lot of time in WF2.



Here is a list of reasons to upgrade for more leverage:



http://www.ptc.com/community/proewf3/newtools/index.htm



The biggest benefit I have seen with WF3 is the inclusion of the cutout
features in sheet metal parts. I have used them to create
libraries of cutouts so I can quickly turn cuts on and off without ever
needing to open the sheet metal parts. I use skeletons to be sure
everything stays in their proper locations, then use relations in the
cutout parts to control where and what extrusions come through the
sheet metal parts for cutout. I could nto have done this prior to
WF3.



If you use sheet metal for most of your work, there is no reason I can
see to wait for WF3. It is stable compared to the latest build of
WF2 and light years ahead of Pro/E 2001.



Good luck,

Jim