I need some help from all of you.
I'm, with some friends, creating a new company, where we will develop metal stamping tooling (progressive and transfer dies). We are evaluating the needed softwares, and the most proper ones from our job.
Today in the company that we all still work, we use NX and CATIA (I'm a CATIA user). But as far as we have noticed, CATIA and NX are truly expensive softwares, and we need to ponder what to use for our new company.
What we are evaluating.
For simulation we had chosen autoform (that's closed)
For cad we have several possible solutions.
CATIA -> Not much probable, due to price
NX -> Not much probable, due to price
Creo -> interesting choice, but there is some lacks. To create metal stamping layouts, determine the pre cuts, make some quick analysis to metal stamped parts, there is not enough good tools. But for modeling and general surfacing, looks really powerful. Price looks reasonable.
Cimatron -> Very nice to determine the pre cuts, make some quick analysis to metal stamped parts. For 3d modeling there is plenty of libraries for metal stamping tools, But we don't know much about their capabilities to Draw. Price we still don't know.
ZW3D ->Very nice to determine the pre cuts, make some quick analysis to metal stamped parts. Interesting modeling options. Very low market share. Really interesting price
VISI ->Very good to determine the pre cuts, make some quick analysis to metal stamped parts. Interesting morphing capabilities to prevent spring back. Looks good also in surfacing and in general preparation of parts surfaces. It doesn't work with individual parts, it's parametric philosophy it's to limited. Price we still don't know.
SolidWorks -> we have tested it and there is a few things that we have disliked it, so it's not in the equation.
SolidEdge -> we have tested it and there is a few things that we have disliked it, so it's not in the equation.
Autodesk Inventor -> we have tested it and there is a few things that we have disliked it, so it's not in the equation.
Looking to our resarch, there is not a software that can provides a powerful choice for every area that we will need. So we are open to have 2 softwares for diferent needs.
Visi + Cre
Visi + Cimatron.
What do you know about these softwares, and their capabilities for this type of work?
Do you know any other softwares that can fulfill our needs?
If your new company is only developing the stamping tooling, do you have prospective customers to supply the parts and do you have a company contracted to use your tooling to stamp the parts? Are you manufacturing the tooling you design or subcontracting the machine work?
One thing to consider is the CAD package of your customers. How much translation do you want to be doing to bring in their models to your system. If you are not on their system of choice, will they provide STEP models for you to import. NX and Creo have builtin translators, for an extra charge, so you can read native files from other CAD systems.
For now, we will only concentrate to develop the design of the tools. Later we will analyse to expand our business and mill, assemble and make the try outs. ou tools.
From what we have been discussing with our potential costumers, we can provide them a STP file.
Yes Creo, NX, Cimatron (Not for all of file types), ZW3D, are able to open files from other softwares.
For what it's worth, I'm a draftsman for one of the (if not "the") largest tool and die companies in the world. Creo is our primary CAD software, but we also use AutoCAD for legacy files.
Can you name the company?
And for blank generation, springback, formability... What do you use?
The general templates (Standard parts, for ex: Gas springs, Guide pillars, guide bushes... from Fibro, strack, misumi...) What do you have? Did your company invested on created those components, or do you have any thing were you can arrage those components?
You have now made multiple threads about this topic on the forum, and you have received a good reply in the other one. I can also see from your questions you dont have a lot of experience. Let me sum it up for you:
SW or Creo, both are plenty capable for die design on their own-without add-ons. There are specific add-ons for each, Logopress for SW and PDX for Creo.
Now, if you are a long term user of Creo, than stick with Creo. If you are a long term user of SW, than stick with SW, duh. If you havent used any of them, than go with SW. Because Logopress has the fantastic capabilities for unbending, flattening and making a blank. You import your .stp or. igs and within minutes you can get a blank for relativly complex part. The down side of this addon is the price- it is very expensive.
PDX I wasnt impressed with.But I also dont use EMX for molds, so maybe thats just me. I think Creo has enough capabilities on its own, so there really is no need for addons.
But here's the thing. If you cant make design without the addons, you're really not ready to do die designs anyhow. And how everybody does general templates for standard parts is like this: you model them. You take the catalogue and start working on family tables in Creo. Or configurations in SW.
1. With macros I dont have experience, so I cannot help you with
2. Both have a library of standard elements, with option of adding them or making your own. As far as i remember, Logopress has way bigger library thou, but it comes at a price. I sure wouldnt't buy the whole package, but only unbending/flatteting module (you can buy diffrent modules-unbending, strip, die design...do your research). I wouldnt worry about standard elements, I would be thinking more about the making of the blank and strip.
3. There are many approaches for making features from part level to assembly level and vice versa, you need to be more specific in what you want to accomplish.
I was never trained by PTC and neither were my coworkers. What we have, is a reference skeleton based parametric die that contains all the standard parts based on family tables. This was all modelled by us, and we are upgrading the assembly as we go. All the main features are already made inside the parts, so it is only a matter of supressing/unsupressing and changing values and references. It works well for us.
- You simply assemble your pillar, than you make a cutout from all the plates with this pillar-->component/compnent operations/cutout. I probably dont need to tell you that is a bad idea.
- A little better solution would be to extrude a surface of the diameter of your pillar in the skeleton part. Than you activate each part you need to make a hole in (ie plates) and use solidify feature.
- Far better solution is to make a sketch in skeleton part with points (ie coordinates of the pillar position). You also make an axis on the first point of this sketch. Now pattern can be used for features and mates.
You just activate the plate,use feature HOLE, click on the axis in skeleton and perpendicular surface on the plate. Than you click pattern/by sketch and click on the sketch with points. Now you can make multi-diamater holes with threads or clearance holes for punches and bushings all in a couple of clicks. You can change the number of pillars from 4 to 40 by just adding the points in the skecth in skeleton. Just click refresh, and all the pillars and holes on all the plates will be added in your assembly-because you referenced the same sketch and used pattern.
You can use UDF (user defined feature). These are custom features, that you can save and use at will, for example: 40 diamter hole 15 mm deep with M8 thread. You save this hole as UDF, and you can use it than as a regular hole (feature), so you dont have to insert values everytime.
When using solidify feature, the faces of the cutout will be the same color as was the surface that was used to solidify. So you could have multiple surfaces of diffrent colors to achive diffrent color pockets.
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