Every so often I receive a customer file like the one attached - with no attention paid to weld seams. I would need to convert this to at least 2pcs maybe more to make it easier at the brake, all the while closing the corners so as to be suitable for tig welding. How would others handle something like this. On this one, I have 15 or more steps in trying to close the corners and split the part. Is there an easier way.
John,
It is amazing how stuff like this rolls downhill and lands in the manufacturers lap. If an engineer is going to design sheet metal parts, it would be nice if they had some real world experience in manufacturing first. It is obvious the engineer who designed and modeled that mess is either oblivious to the issues he or she has created or just flat out doesn't care....(somebody else's problem). When I see stuff like that it makes me want to slap the engineer upside the head.
Bob
I agree that is bad modeling,
I would create a dummy assembly place the STP file in the assembly and
re-create the part with your workflow and re-model the new part on top
of the old one using the old part as reference. Save the new part and delete the assembly.
Frank
I was able to close up the gaps to something acceptable to the welder, by converting and using closed corner repeatedly. I've tried other ways, some of which has been mentioned, (thanks), but was hoping/looking for a chance work around that could close and fill, kind of like delete face and patch. Thinking I'm stuck with the current schemes.
John Christensen wrote:
- with no attention paid to weld seams. ...
I would also request a 2D drawing with finished dimensions.
I measured some of the distances between faces and wonder how much attention was paid to dimensions.
Be sure that you write the contracts to get paid to fix their models.
The geometry itself isn't too terribly complex to recreate from scratch, but if the dimensions don't make logical sense....
John,,, When I get a file this bad I do remodel it similar to how Frank suggested. Only difference is I did this in the part environment. Created a base flange on top of your part (No Merge) and did a series of edge flanges, edit profiles and used collinear, parallel, relations. I also used the parallel to face option for the edge flanges (off of the imported model).. I hate to say it but I think this is the only way to get a decent model. As you can see the edges (corners) are ripe for welding and you get a good looking flat pattern. You should also add some bend reliefs in order to make this more laser friendly. If you punch it you are going to have to live with some gaps. J mentioned the dimensioning and I agree. I thought perhaps this was supposed to be metric since some dims came out good round numbers (including the bend radius) but some carried out 8 decimal places (probably to infinity). Whether decimal (inches) or metric. Something is goofy and as J suggested a drawing would be helpful and you indeed should get paid for fixing this. I used a Body-Delete/Keep on the imported model in order to view my part more clearly. You can suppress that to compare the two. For me who has done this sort of thing many times it took me about 20 minutes so, unfortunately, there is work involved.
The cover is for tool and die-set components, so the size is per component placement and rounded to 1 or 2 places. I do usually have prints, but they are built around fitting to the die-set, and not sheet-metal modeling and fabrication. I get the feeling that the designer knows die design, and only roughly details the sheet-metal work, then passes the additional work (and costs) off to the vendor. They are usually only one offs though, so the lot charge does cover that. Thanks Dennis for the clean and concise model, and also the straightforward methods for getting there. It's always a shock to see incoming work like this and easy to get into a "you've got to be kidding" mental block to just simply starting over. In the end sometimes that seems to be the best method and produces the best work.
Oh , come on.
It just needs a little wire.
One way to do it with a few features is use the un-fold feature, then add a sketch to the areas you want to extend, extrude to the thickness and re-fold.
You can try the close corner feature, but thinking with all those angles and different offsets etc, might be a challenge. Sketching may take a little longer, but you should have positive results that are easy to modify...