We have a new customer, and at the moment they are supplying their full assembly model with all the .sldprt and .sldasm files. I've not gotten the chance to visit with the customer and help make this work the best for both parties involved. But, I have plenty of questions for you that have/do work with similar projects.
I thought I'd be "smart" and open all their 100+ assembly files and save them, thinking that would give me all the associated parts converted and ready to go. Now I have multiple versions of the same parts, and they are all .par files. We like to use that macro that calculates the total cut length, and kicks out a flat pattern .dxf file. Well, it doesn't kick out .dxf files when it's a .par file.
I have started over, and opened their part files into a SE .psm, and most of that has gone well, but I've run into one part that doesn't have correct bend reliefs, and I have to finger out how to get that fixed.
Thus far I don't have a BOM or any material specifications, and I plan to address that with the customer, but thought maybe I could gain a little more knowledge of other things that would make this work in the simplest manner. I've considered installing a trial version of SW, but have a few fears that it might conflict with SE if it's on the same computer.
Words of advice? Maybe I'm just stressing out and need to take a few deep breathes...........
Does your customer's SW assemblies and parts contain configurations? This might be why you are getting duplicates in some situations.
Solid Edge does have a SW Data Migration utility that can be used to help bring over the data more "intelligently". File Properties, materials, assembly relationships, "configurations" (or families), etc. The catch is you have to have a seat of SW available for the utility to communicate with (on the same PC or same network).
You can still do what you are doing and just do a File-Open and do a lot of what is described above manually but the utility definitely gives you additional benefits.
Thanks for the tip! I'm running it now, seeing what sort of results I get. We don't have SW installed, and don't have any intentions at this time.
So, it created all these x_t files, I can open those with SE view and markup, looks great. How do I convert those to sheetmetal parts now? If I look at the individual part properties in the view and markup, it's all in metric, but the models are actually done in inches. Is there one more step that I'm missing?
If you don't have SW available (on your PC or access to another PC that has it installed on a network), you may not want/need to use the Data Migration utility. That utility provides more benefits is you are using it in conjunction with a seat of SW.
You may want to stick with File-Open.
In Solid Edge Options-Helpers-Set Default Templates, what are your templates set to? If your default templates are metric, you might want to switch those to ANSI or other "English" template so that when you open the SW assemblies, the subs and parts will open in the template specified.
My templates are ANSI(inch), open files I'm fine, for some reason the view and markup was showing me metric.
I guess this converter might not be of much help at this point, but thanks for the information. If I open the x_t files within SE, it also creates all the parts inside the assembly to .par files, when most should be .psm files. I'm not sure the "best" way to move forward. I guess I have to open each sldprt file and make it a .psm, and then open the sldasy and save all those .par files, and then replace with the correct .psm files.....................
That's why I'm asking for suggestions! Doesn't seem like my current path is the best.
Yes, you could open the SW parts that are supposed to be .psm and then replace them in the assembly after conversion. If you don't care about the file name having a .par extension but still want the geometry to behave as sheetmetal, you could open the sheetmetal .par files and under the Application button select Switch to Sheetmetal. Once in the sheetmetal environment, you could Transform the part to sheetmetal under the Tools tab. If truly a sheetmetal part, it will be a sheetmetal part but with a .par extension (I think).
you will run into the same problems I do modeling sheet metal in ordered. Since I don't use Sync yet, I cant say if it has the same problems.
Back on point, it can be impossible is get SE to create some specific flat patterns from a bent up model. Two models are required. One that can be bent, and one that shows the dimensions of the finished part.
When you translate from any other software, I would expect there to be situation where the sheet metal part will not be able to created the same flat because that flat just simply cant be created is a manner that folds up in solid edge. I'm in process of a 30+ ER process that addressed mainly that issues.
"I guess this converter might not be of much help at this point, but thanks for the information. If I open the x_t files within SE, it also creates all the parts inside the assembly to .par files, when most should be .psm files. I'm not sure the "best" way to move forward. I guess I have to open each sldprt file and make it a .psm, and then open the sldasy and save all those .par files, and then replace with the correct .psm files..."
I understand your painful, but don't worry there is a solution. You have to copy from your psm template and rename it from .psm to .par. Setting it as a default template file and open your sw assy.
All sm parts will be in sheetmetal environment but with .par file extension... You can rename them to .psm if you want with Revision Manager, but not necessary...
Here are steps: