Tough (but should be easy) question in Pro Mold

[pimm]

I almost have a die complete in Pro Mold.

I only have one problem, and that is that I can’t seem to move the imported solid objects which is important.

In our industry we have to mismatch the top die impressions independent of the bottom die impressions.

If I do a copy and move of the solid component for the top die it attempts to keep both of the solids. I can’t remove the original solid by hiding it. I can’t delete the original solid without unhinging the die model.

I just need to offset the top impressions and get rid of their original location in the top die.

Would you have an idea of how I could accomplish this?

It appears that you are stuck with the original position that you import the reference model. If there isn't a work around for this problem which should be simple I'm afraid ProMold is going to be worthless to us. There must be some way around this.

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[James62]

Hi Paul,

I've always thought that Pro/Mold is used just to lay out core and cavity as a foundation for the rest of the mold. That means the rest of the assembly just inherits what's necesarry, and that way can be the mold assembly used sort of like a skeleton model.

Simply put, if you need to make some extra impressions, then make a whole new part that copies the core or cavity and simply borrows the shape from mold assembly,

Leave the mold assembly as surface volumes, and make your own solid parts of of those, which you can freely edit then. You don't have to use the mold package to create solids from volumes.

Also, to move one of your imported objects, copy it's surfaces to another part, and then move those surfaces wherever you want with copy and paste special.

What version of Creo or Pro/E are you using?

[pimm]

Thank you for your thoughts on Pro Mold Jakub. I can see this package in the way you describe it.

I just received some assistance with what I'd like to do and the individual who helped me described a method similar to what you suggest. Perhaps I can follow this path but it is quite difficult based on the method I have become accustomed to with ZW CAD. There are some reasons this methodology is difficult to embrace:

1) All I need to do is move a couple impressions in the top die. Based on what I've already experienced there should be a 30 second solution to this problem (just use the move command and move both impressions to where they need to go).

2) I don't like tracking and keeping extra files. If I inadvertantly lose the extra file (which I've already done in Pro Mold) it likely would mean redoing a lot of work and possibly introducing a costly mistake to the shop floor.

3) The parametrics to make a change are a lot looser. You would have to control the model from different part files.

4) To have an independent top and bottom die you can't be sure you won't have unintended collisions between die halves.

If it wasn't for the issue of dirtying data with translating IGES or STEP it would seem to make sense to drop the far more expensive ProMold license and just do all the die work in ZW CAD. The ProMold tool appears to just add time, complexity and a greater likelyhood of making mistakes.

Perhaps I've missed the better features of ProMold, but for crying out loud, I just need to move a couple impressions. I am hoping that the developers might listen and find a better way of interfacing the inserted parts.

I really do appreciate hearing feedback from someone who does use the ProMold software. You've already gone through the struggle of determining what works the best in your situation. I don't know what the options even are. I'm still really hoping that by doing somewhat of a paradym shift on my end I can find a very viable way of using the ProMold software.

I have tried making the reference part as a surface model as you have suggested. My die halves are quilts without impressions. This idea should help me subtract out parts in the position needed. When I select the die and the refererence quilt to remove the impression I do not get the merge option. I'm so close to a solution; I'm not sure why this doesn't work because other merges that I've done with quilts and the die do work. Any ideas?

Thanks a lot for your suggestions.

Yes; and my version of Creo is 2.0 release M90

[James62]

Ok, so you are on Creo Parametric 2.0. That's great.

Just to let you know, I don't have the Mold Design extension, it is just waay too expensive for what it offers. I've only had borrowed licence for about one month about two years ago, and then I studied it alot, but after a while figured out it adds almost no value to my workflow.

I make alot of unusual (atypical) mold, and this Mold Design or TDO extension fits mostly for molds for thermoplastic parts, and well, I am not the lucky guy who only makes simple molds for thermoplastic parts, so TDO is kind of useless here.

The only nice function that TDO has is the shrinkage, which happens to show in feature tree, and also that it can be an anisotropic shrinkage that you can simply roll-back, that alone is really nice. The rest of the features are just replacement for tools that are already there in Creo Parametric.

Now, for anisotropic shrinkage I just use Rhinoceros, and the rest of the work I happen to do in Creo.

One thing I'd recommend is to use it while you have it. Does it split the core and cavity faster than it can be done in ZW CAD?

You know you can convert features into an imported feature using Collapse Geometry? That might be a way how to get rid of your "skeleton" models in case you don't tend to keep them, but there is one thing you should always remember, and which will save you tons of time once you will be making some really complex molds. That is parametric modeling is alot like programming. You really should split your code into several files, and do smaller chunks here and there. The recommendation is always to be as descriptive as you can be. It makes designing and design changes easier when you can just replace some parts with others.

One skeleton with 500+ features/datums is just bad idea. You can always introduce layers to these to give them sense, but that's just too much editing kind of work.

I use Collapse Geometry to break links between parts or skeletons pretty often, and also to get rid of circular references. If you have Flexible Modeling Extension you should have no problem editing dead data. With AAX and FMX it's not that hard to recreate the parametric links between parts where they are necesarry anyway.

About merge, if you have the quilt you want to subract from your solid model there with your solid model on part level then you can just use solidify to cut from it. Or you can turn the solid geometry into a quilt using remove feature with the options "Leave open" and "Keep the removed surfaces".

Try to check these options in Remove feature dashboard. They might not be there if you don't have FMX. In case they are there then, well, that should do the job.

[pimm]

Jakub,

I appreciate your description of how you pull things together in your work application. I can certainly relate with you in that the most immediately appreciable aspect of Pro Mold is the shrinkage. In our case it is just having a feature in the tree that shows the shrink that was added. Our shrink factor can change so it's good to be able to review this value; also having this in the feature tree is somewhat of a goof proof to make sure shrink was even added. We don't used anisotropic shrink, even though it might make sense in certain applications. We are used to not having this control so some times we will change the models length to essentially get an anisotropic type result. Perhaps this is something we will get into more.

In what we've experienced so far ZW is much quicker with core and cavity subractions. We really don't need a special interface for this as ZW doesn't have a 1 solid rule. With ZW you can keep both sides of a split even though you have depth across the parting line. You don't have to abandon the use of solids with your impression models (reference models) as you can decide when to make moves or order dependant subractions. You don't have the extra merge commands which are necessary when you work with quilts. The ZW feature tree in a die would be much shorter. With all that being said I "know" there have to be tricks that would speed up die creation in Creo.

I'm not really familiar with the terms "collapse" and "skeleton modeling". I thought "skeleton modeling" was only possible through AAX. Through my years of die modeling experience I have learned to take advantage of componentizing models to make complexity much more bearable. We will make independent files for impression related flash, the impression itself and these models assembled together. We will drop the various impression assemblies into a die so all that needs done in the die is the transitions that are part of the die itself.

It may be that "Collapse" and "Skeleton Modeling" would be time savers for us; I'd like to get more familiar with this. I thought that "Skeleton Modeling" was just building a set of datums knowing how typical models are created and saving this as a template file.

Flexible Modeling would be an intriguing package to have, but it's probably not in the budget for us.

I was able to resolve the "merge" issue. I didn't realize that you could just subtract quilts from the die volume quilts using the die volume split option.

I will have to try the Solify command with a quilt that gets merged into a solid. That sounds like a good method.

Thanks for your ideas!

[James62]

Skeleton model is just a term for a set of surface groups and datums, it doesnt need to be one from AAX. To design a mold cavity, it makes sense to work just with surfaces and quilts, and make the solids afterwards. All I am trying to say is that you don't need to bother making solids from volumes directly in MoldDesign.

You can design the core and cavity, and then bring it to another assembly just as it was a skeleton model. Copy the volumes from it to another parts, make some changes using FMX, or the not so favourite Copy and Paste Special approach, and there you have your completely custom mold.

Collapse Geometry can be then used to break the dependencies between MoldDesing assembly and your actuall mold assembly to which you also add plates, etc. You can create Independent Geometry features to which you can collapse whatever solids, surfaces, curves that you don't want to be parametric, it doesn't have to be an Imported Feature.

I am not sure if it's possible to use FMX commands inside MoldDesign module. It sure can be used in the regular parts that would copy these MoldDesign models.

I also use Style feature alot, for which ISDX is necesarry. This one offers even more freedom, from which the MoldDesign module can also grab surfaces for parting geometry reasons.

I just wish all of these modules were at least abit similar, it's not easy to learn all the ways to build a mold or whatever assembly in Creo, but there sure is enough ways to make whatever you can imagine without using another CAD platform, it just often takes more time, but then changes are alot easier to do.

From what you wrote so far here, I guess your best bet is to propably keep ZW, drop MoldDesign module, get trial of FMX, get to know how to work better with IDD You are gonna need IDD for taking the core and cavity from ZW as imported features.

I am all for taking stuff from here and there (CAD platform wise), and putting it all together rather than remodeling things from scratch. This whole approach just allows it. Imagine you have a cavity modeled here, and some old mold base or frames there, and you can just put it all together, reparametrize what you need, create drawings, and use all this bunch of files as a template for any new mold you are going to create. This is what they call Hybrid Modeling, not something easy to learn, and not as straightforward, but surely an approach that lets you get rid of alot of duplicate/repetitive work.

[Inoram]

When you say mismatch the top, do you mean, just pull it away some?

[pimm]

Hi Matt,

With the term mismatch; in this case it refers to the reference part impressions being moved in the X direction in the top die only. This position leaves a small stagger between top and bottom impressions.

[dschenken]

I would think that mismatch is a bad thing, at least when I get a plastic model kit with mismatch, the smaller parts are often useless - it appears to have a valuable use, but I'm not getting what that use is. Any description for why it is good to add it?

[pimm]

David,

This might sound funny but in our industry with multi impression forging dies we add mismatch so we don't have mismatch.

The preforming impressions are not on the center of the die, because of this when the ram hits the billet it hit's it off center. Since it hits off center the impressions do not line up naturally, henceforth the need for mismatch. Our finished part however is lined up closely to the center of the die so that impression doesn't need mismatch.

We have a very basic work environment but there are some extremely challenging aspects in designing dies.

[dschenken]

This accounts for deformation/deflection of the die/machine during the die forming process? Make sense.

I came across some analysis software that is dedicated to FEA of forging and other high-deformation methods - QForm from FIT. It didn't mention processing equipment deflection, but who knows?

"QForm was originally designed** for the simulation of hot and warm closed die forging and it is ideally suited for this process. The software accurately shows material flow in the dies and predicts defects such as voids, laps, and flow-through defects as well as stress and wear in the tools."

**They also do a lot more; hence originally designed.

[pimm]

Yes; the ram deflects and because of this we have to have mismatch in our top die impressions. (Which is turning into a pain in Pro Mold). I guess as a CAD developer you can't account for the many different ways the software will be used. Some software has more flexibility than others. 1 quirk and you end up with lengthy work arounds.

I've looked at the QForm simulation software but we use DEFORM.

Unfortunately there is no easy way of modeling die deflection in DEFORM (or other similar FEM packages). The deflection issue certainly shows variations between shop floor and our predictions. Once again this same quirk causes a lot of pain.

[dschenken]

I wonder if the Flexible Feature Module would help. You really just want to shift the entire cavity; it's about as direct-modeling as one could want.

As an aside, it bugs me that the deformed geometry from, say, Mechanica, wasn't available as a model surface, to use for compensating for such conditions. Being able to apply a blanket of offsets from the deformed model would be useful.

[pimm]

Just curious in what Flexible Modeling can do:

1) Can this be used while you are in the Mold application?

2) Can you move solids with Flexible Modeling?

I discovered that I can't even move reference model quilts when in ProMold. I ended up having to bring in the same quilts in a different position.