Sheetmetal Difficulties - Can you figure it out?

[SamLamb]

Hello all,

I'm trying to recreate a part in Pro-E Wildfire 4.0. I've attached the .prt file that is from a step file. How can I make my own in pro-e using one piece of sheetmetal? I've tried just about everything but to no avail (deformation area, mirroring, solid-convert to sheetmetal, just sheetmetal, etc.). If you have some free time and would like to try and figure this out, please let me know how to do it! I'm stumped and very short on time with this project.

P.S. It has to be able to convert to a flat pattern so we can get this manufactured.

Thanks,

Sam

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[dgschaefer]

I would think this could be modeled as a solid with radii at the top edges and then converted to sheetmetal by shell. Then, add a conversion fearture to edge rip the sides. You'll need a very narrow cut down the one face from the shallow peak so it can unfold properly. Then you can add the walls needed for the bottom return flanges.

Good luck.

[SamLamb]

Thanks Doug. By narrow cut, do you mean remove material by using extrude? Also, you're saying put the radius in the top edges of the peak before conversion? If I could just get the top and sides figured out, the bottom flanges would be a breeze.

[dgschaefer]

The side that looks like one piece and has the peak at the top would have to be split in order to unfold. After converting to sheetmetal, yes, I think I'd create an extruded cut to remove that material.

[TomD.inPDX]

That almost looks like an outdoor utility enclosure roof.

You need to have one question answered by the fabricator. Is the center seam along the crown going to be welded and ground?

The way I see this modeled ...and fabricated, is to make the "kink" in the large top surface last creating a seam in the center of "front" and "back" flanges which will be welded and ground.

So what this means when modeling the part is that you need to account for the odd angles for all the bends. You can add the holes after you finish that shallow-angle bend in the top if that makes things easier. This should unfold without issues using this method.

[TomD.inPDX · Accepted solution]

A good afternoon's excersize...

...and "The Movie":

Video Link : 3917

I must be getting better at the sheetmetal module. This was easier than anticipated.

I'm sure a few features could have been simplified but in all, 72 features with welds and unbend/rebend. Not too bad. Any sheetmetal poweruser tips welcome.

Creo 2.0 and STP attached:

[SamLamb]

Wow thanks man! You make it look so easy. I'm comparing your step file as I'm making the part and I'm stuck at the 4th step where you make the 3rd wall. I just can't seem to match up with what you have for the relief on the left side. I'm guessing its a rectangular relief but I can get the wall to come out flush with the left wall. Any insight on how you did this? I bet this is a whole lot easier with Creo 2.0! Let me know if you get a chance.

Thanks,

Sam

[SamLamb]

Nevermind, I just figured that part out. I know I will have a question with the last bend for the roof so I'll ask it now: What did you do for reliefs on the center? It looks like an obround relief but did you have to take the space between the two walls that come together into consideration before making the last bend?

[TomD.inPDX]

Those are the notches I put in with extrude in the First Wall.

Sam Lamb wrote:

...What did you do for reliefs on the center?

...

[TomD.inPDX]

Yes, I modeled a new planar sheet and then Joined it to the First Wall.

I filled in the small gap (0.120) with a straight wall at "flat" (#19 and #22).

I find there are a lot of limitations with clean bend relief's when you try to minimize gaps. If you try to do this with extrudes, you loose unbend and bend-back capabilities. If you try to sketch a good bend relief when building flat walls, the system either fails or ignores you when you do something within the bend. The unfold flat pattern is a bit more robust, but always being the last feature, I never like leaving the master rep as a flat part.

There is a small step you might not see clearly in the video. #10 and #11 are small notches (extrudes) in the First Wall to break up the front and back edge. If you don't do this, you will have trouble building subsequent walls on the same edge.

In retrospect, I realized I could do many of these walls with sketched Flat walls where I used flanges or new planar walls later to be joined.

Good luck with your project!

tom

[SamLamb]

Tom,

I'm having issues with the last roof bend. I've never used the "insert bend" function before but I tested it on a regular flat piece of sheetmetal and it worked just as I had figured. For some reason, when I try it on this piece it keeps telling me "could not construct feature geometry". If you open the part I've attached, obviously I'm nowhere close to being done but I wanted to make sure that bend would work before I get everything else done. Do you know what I'm doing wrong?

Thanks,

Sam

[SamLamb]

After looking into it more, I can bend an angle down to 5 degrees, any angle less than that it won't do.

[SamLamb]

Ok, well it can bend down to 3.5 degrees but thats not what I need. Also, what is this join command you are using? I'm guessing its "merge wall" in WF4.0 but I have no clue how to use it. Argh I'm not a big fan of sheet metal anymore.

[TomD.inPDX]

Sorry Sam, I went for a nice long bike ride today.

When I put the 1.5 degree bend in there is didn't fuss about it. I made sure I had good clearance for the two mating walls.

Maybe try putting the 3 degree bend is just after the notches (2x 1.5 degree)?

I will take a look at your model later and see if it works in Creo 2.0.

[TomD.inPDX]

This one threw me for a bit but for me it was just another default accuracy issue.

When I opened your part, the accuracy was set to relative and .0012. Pretty much the Creo 2.0 default. And pretty much a cause for many issues when making larger parts.

I have this in my config.pro: enable_absolute_accuracy yes -and- default_abs_accuracy .00005. When I open new sheetmetal parts, the accuracy settings come up with absolute and 0.00005. Your 1.5 degree bend works fine in your file even with 0.001 absolute accuracy. Funny though; new solid part files open by default with relative .0012... go figure! Accuracy is set in Model Properties in Creo 2.0. Now sure where that is in WF4... but you need to set the "enable_absolute_accuracy" to yes in the config options to invoke them in the model properties.

You might also see if you have this in WF4: minimum_angle_dimension .1 (1.0 by default in Creo 2.0!)

According to the WF4 config.pro options, you have access to all 3 of these options available. That should solve your issues.

[BrianMartin]

In Wildfire 4 it would be under Edit->Setup->Accuracy.

[SamLamb]

I got it figured out. The accuracy was the problem. What a eye opener that was! Thanks for all the help!

[BrianMartin]

Hi Sam...

Antonius' answer to this geometry is certainly valid. However, I'd encourage you to take another crack at the technique suggested by Doug Shaefer.

Hands down the best feature in sheetmetal is the Conversion feature. You can create most of the geometry you need for this model as a regular Creo solid that's been cut and shelled to the proper thickness. I haven't taken a very deep look at it... but I believe you can create this entire model with regular Creo features and less than 5 sheetmetal features.

I also think you can do it with better dimensional control in about half as many features. The Conversion feature is one of those best kept secrets that can really save you heartache when working with sheetmetal objects. Let me see if I can work up and example and post it.

I'm not saying Antonius' method is wrong. There's no doubt this technique works and uses pure sheetmetal functionality throughout. While I like working in sheetmetal, I find I like to use basic Creo modeling when I don't absolutely have to use sheetmetal. I have a similar philosophy for piping and cabling applications.

Good luck!

-Brian

[TomD.inPDX]

I have gone through that training module for the conversion before. It is indeed powerful. I suspect the corner reliefs would be easier too. Corner reliefs are the only real problem I run into using sheetmetal.

I reversed the process I used before by doing the 3 degree bend 1st, then using sketched flat walls. It made the whole process much simpler cutting the number of features in less than half.

I'm looking forward to seeing how you do the inward flanges using the solid shell, Brian.

[BrianMartin]

Hi Sam...

Here's what I was talking about. I did not add the holes. I figured we can all agree on how to add those. Personally I'd probably go with a pattern on point but that's irrelevant to the sheetmetal stuff. Here's the bent version...

And here's the unbent version...

Notice how short the model tree is. I did use 11 sheetmetal features so I was over my guess of 5. The odd bottom angle necessitated creating some split surfaces to enable the rips required for unbending. I can get the number of sheet metal features back to 8 but I decided this was probably enough to demonstrate the technique.

I'm attaching the file in Creo 2 format. Take a look and see what you think. One of the main benefits of this technique is that you can specify the height, length, and width of your model all in the very first feature. This means everything can easily be model driven.

Thanks and good luck!

-Brian

[TomD.inPDX]

Very nice, Brian. Those V-notches on the backside failed when doing this in all sheetmetal mode. Yet the corner relief's in the front did work better. Some improvement in tweaking corner relief's would be a good thing.

[BrianMartin]

Did you get a chance to check out rhe conversion feature? It gives you the ability to add bends, rips, and relief all at one time. If you plan carefully, you can build a very simple model using basic Creo commands then switch over to sheet metal and perform essentially all of the necessary commands to 'unzip' the solid at one time.

Think about what we start with. In the first two features we're able to incorporate the height, width, and length of all sides and all but the front/back flanges. Were it not for the angled bottom, we very well may have been able to create the entire piece in just a handful of features.

I used some Split Surface features (these used to be Deformation Surfaces). They simply allow you to break up one large sheetmetal surface into smaller surfaces. Before the advent of the sketched rip, you used a deformation to generate edges which could be ripped out with the edge rip feature. This technique still works. I still think I prefer it to the sketched rip for some applications.

Anyway, there are obviously other solutions that work equally well. This was just my take.

Thanks again...

-Brian

[TomD.inPDX]

Yes, I looked through your model. It is a very comprehensive conversion. I will have to play with it more on future sheetmetal parts.

[dgschaefer]

I'm glad you were able to post this. I was hoping to come back and give this a shot and post a model, but never got the time.

I've had great success starting with a solid and converting to sheetmetal. Unfortunately there's some kind of stigma against this, we have some clients that prohibit starting a sheetmetal part with solids and converting.

[BrianMartin]

Hi Doug...

The only way I do sheetmetal parts is by starting with a solid and converting. It's our "best practice".

As for the stigma associated with it, those clients need to be educated as to the benefits of this process. In some respects I miss commercial work. It's faster and very competitive. I love that part about it... every dime counts, every minute counts, precision counts... and the client rules.

In my current line of work... we can do things the right way. We're the client. There's less competition and the pace isn't always fast. But universally I can make the case to do something the "right" way and win. When you're dealing with a client who doesn't always understand the software, educating them and changing their mind is sometimes a futile endeavor.