Calling all weldment experts

OK I'll try this group also, please please stay on topic!
My company manufactures material handling equipment (lifts which personal
can't ride). They cut, machine and weld up a bunch of structural steel, paint it and assemble purchased components to create product. See www.pflow.com for further information. There has been a push to implement Solidwork's weldments package because the cut lists interface well with DBWorks. After playing with the add-on for about 2 hours, I can't get it to do what or how our shop fabricates weldments. I've known about a few shortcoming, but I've found a few more since my little experiment. I could be missing something since I've only have the 2004 training class on weldments. Here are a few of my findings, please correct me if I'm incorrect.
1. No gap can be created between joining pieces for shop fit up. Structural steel is hot rolled from the mill and the tolerances on the OA heights and flanges can be quite generous (5/32" height wise and " on the widths). I typically cut back 1/16" on all steel butting against a flange and let the fabricator fill the joint with weld (obtaining better penetration also).
2. Many of the weldments are orientated to the top side, to support the load; it must be flush with a plate on top for ease of loading with pallet jacks and fork trucks. Since we optimize materials for strength vs. weight, many times the internal members are smaller than the external structural members. I cannot shift the internal profiles to match the top side without multiple sketches on multiple planes or multiple profiles offset at different heights.
3. Unlike structural steel parts created with sketches and features, I can't suppress filleted edges in weldment profiles. I typical create configuration with all fillets suppressed to speed up the assembled steel parts or for quicker FEA analysis.
4. Internal member's sizes and lengths are dependent on other internal and external member's sizes. So with weldments, I require multiple sketches to have these members have relationships to other members. These extra sketches must reside below the referenced members in the feature tree.
5. We don't cope steel as complex as Solidworks extends faces to another member, we typically just notch a rectangular cutout in the corner to match the flange and fillet in channels and beams. No custom copes in weldments.
6. Parts can't have display states, only assemblies. multi-bodied parts can hide bodies, but not with weldments. How can I show just one of the structural parts which require machining? I was able to detail out the part, but only after hiding the edges of all the other parts I didn't want shown. With display states, I can create a separate state for each part which requires machining. With multi-bodied parts, I can create separate configurations for each part which requires machining. All weldments require some type of machining or modification for stuff can attach to it or it can attach to other stuff.
There might be other issues, but I've only played for a short time. Please feel free to comment or ask questions. I hope to resolve these issues before we jump on board without a paddle.
Keith Streich Engineering Department Pflow Industries, Inc.
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Hi Keith,
Don't do a lot a weldments so can only help you with the first part of number 6. Use "Relative View" to detail the members of the weldment in the drawing and make sure the Scope has "Selected Bodies" checked.
The companies I know that manufacture a lot of weldments don't use the SolidWorks Weldment feature, for the most of the reasons you state, they model them as assemblies. Shame this part of SolidWorks software doesn't seem to have been writen by someone who has much knowledge of welding.
John Layne www.solidengineering.co.nz
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Thank You, this works well. Now I just need a few more issues resolved.
Keith

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Never thought I would see the guy that built the Harley elevator down by the state line on the newsgroup.

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Why is that? I need your input to provide better product more efficiently at a lower cost. I thought that's we all should be doing.
Keith
PS It's not an elevator, it's a vertical conveyor (moves just things), or else the elevator would red tag every unit sold.

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My bad, vertical conveyor (VCS). I guess you can't ride in the hearse on the way down unless you didn't get in under your own power. :) Does the guy who pushes them out into the window use the stair?
BTW Isolate works on my box with weldment features or just multibodies.
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Isolate does not work with multi-bodied parts or weldments. I can hide the bodies though, I just have to create a configuration for each piece which requires machining.
Keith

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Keith,
Maybe I'm missing something because I have no problem using isolate in any multi-body part with or without a weldment feature in SW2008 SP2.1 and higher.
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Maybe I'm the one missing something SW2K7 SP5.0.
Keith
PS We have not jumped to SW2K8 for fear our ERP / DBWorks / DriveWorks will not work together (even though the last two are gold partners and our ERP will never be even a tin partner). Basically our ERP is an old UNIX system migrated over to windows with ODBC capabilities and our to go guy has been working on a linking API for two years and upper management steps very carefully which surprises me their are devoted to weldments.

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I can tell you dbWorks will work with 2008 although there were some hiccups at first. I was running this 200+ body part through it.
I can't tell you about DriveWorks or your ERP although I would suspect dbWorks handles the ERP side so if dbWorks is OK with it the ERP should be too.
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Keith,
1. You can try creating custom weldment profiles to suit your reqs. This will affect your cut list lengths though. You'd have to sort out the pros and cons for yourself.
2. Might want to try using separate sketches for each profile type. (sketch1-4x4 only, sketch2-2x4 only, etc). see #4
3. SOL, the fillets are integral to the profile.
4. Personally, I put all my sketches at the top of the tree, then the members, then the trims, then machining ops. Seems to work out well for me. This method will require sketches to reference other sketches rather than members.
5. Try breaking large weldments into smaller sub-weldments and bring them together in an assembly. Sort of a best-of-both-worlds.
6. A detail view or separate sheet for said part would be my first thought as well. Although convenient, I shy away from multi-part bodies and mirrored assys, parts and features. Call me old-school but they always seem to bite me in the ass down the road.
I've had issues trimming to bodies. I always trim to planar faces now.
I think you may want to play a bit more or try a prototype project before jumping in with both feet. In my opinion, you're asking a lot of the welding module, and in doing so, have already found some shortcomings and work-arounds.
Perhaps you are the weldment expert ;)
rod
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LOL, mine are pretty much a dog's breakfast.
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Ok, I've got one more for the group. Is there an easy way to have a design table pick the profile to use for given members? I want the user to punch in "4" and the design table to propagate the appropriate pieces with a C4x5.4# profile. I think there's a hard way to do this, by linking each profile's dimensions to a design table column and having those cells update via a master input spreadsheet. There would only be one configuration, but the design table would drive all the variations of the weldment.

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Keith
LOL - reminds me of a response given a few years ago when someone asked if there's an easy way to design the hull of a ship.
"Click Insert\Boat" I believe was the quip.
It's been my experience that if you can arrive at the numbers you want in the Excel sheet then the rest is easy. Just link the dims to the proper cells.
I used to cost out my machines at my old employer using a fomula-laden Excel BOM. I don't see why you couldn't utilize a design table in the same fashion.
Your Excel-Fu must be good
Rod
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There is a fellow on the SW Forum, M. G. Martinez, who does some pretty amazing top down design using Excel. A lot of his parts are sheet metal, but I suspect you could learn a lot from some of the sample assemblies that he has posted for downloading.
Jerry Steiger
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Hi Keith,
Please keep the group posted with your conclusions on the Weldment functionality.
John Layne www.solidengineering.co.nz
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So far .... Let's take them step by step.
1. A gap can be created by sketching non-conecting lines. A dimension from end point to line can create the gap. Sort of FUBR to have any sketch with non-meaningless dimensions all over to the overall intent of the sketch or weldment.
2. No easy shift in profiles orgins to position members toward one side. A 3D sketch could be creatred to offset the smaller members, but then again you would have a sketch that was crazy looking unless one understood the meaning of these offset lines.
3. Forget about turning fillets on and off. A profile is a profile, live with extended time to display models and assembles, not to mention regenerate drawing views. FEA packages love rounded stuff (so I'm told).
4. Relationships to other existing members. A design tables project from heaven! Yep, can be done, but don't look at my equations.
5. Cope Solidworks way or cope Soildworks way! If your facility can't afford a fancy waterjet, plasma or laser, what are you doing in business anyway?
6. This one way solved, by your "Relative View" and "Selected Bodies" suggestion. Works great! Display states would be a nice touch to weldments though.
Keith Streich Engineering Department Pflow Industries, Inc.
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2. Create some additional points in the weldment profiles to locate from.
You could also use this to solve #1
/just a thought
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Hi Keith, Below my thoughts about your problems:

You can draw your own structural member profiles (just edit an existing profile sketch one and do a save as with another name). Make the new profiles according to the maximal tolerances and the connecting steel parts will always fit and not be to long.

Make your 3D sketch lines at the top side and when placing the weldments use "Locate Profile" to position one of the top corners of the weldment equal to the sketch. Another options is that you can make in the sketches of the structural member profiles extra points (*). These points can be used to locate the profile in the weldments.

Make your own structural member profiles without all the fillets (see 1.)

In the 3D sketch you can make relations between the different dimensions (see Equations).

Do a Trim/Extend to the face of the body of the other member. Second make a sketch with the required cutout and do a cut-extrude (through all). Select the bodies for the cut-out and you have your own corner.

This one is already solved using the Relative view option.
Hope this helps a little bit. Willem
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