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Shrinkage without the use of MOLDESIGN

vonhofs

New member
We have parts that are made at room temp, but are used at cryogenic temps. Because of this, the engineers would like to add another sheet to the drawings, showing the "USE"or cryo dimensions of the parts. These would all be reference dimensions and the sheet would have big notes saying not to use the dimensions for manufacturing.


We are trying to figure out how to do this and don't have any good answers. We would like the models to be dependent on the original models as any changes need to show up on the "Use" models as well.


One suggestion was to do an inheritance model and then warp it in three directions, but that didn't work as it ended up making the holes into strange looking shapes.


Another option would be the simple "scale" command, but we want to leave the original model alone, but have the "use" model connected to it and we cannot figure out a way to do this. I was thinking of making a family table with just different names and then opening the instance and scaling it, but the command is not available in instances.


Anyone have any ideas? If we can't get anything, the easy way to do this is to simply make a copy of the original and then scale it and if the changes to the original are significant, to re-copy it and scale it again (loosing all the dimensions on the views).


Thanks for you help!
 
Use the Warp command, Transform. This will add a feature to your model tree that scales the entire model. This way you can create a family table with two instances, one with (the original) and one without the warp feature. Then add both models to your drawing and create views with each. Dim them up and they should both update whenever you make changes to the original.
 
Would you want to family table the model one at normal temp and the other at cryo temp. Then use the shrinkage feature. Edit>setup>shrinkage.


That is what I would do. What is the shrinkage for Cryo?
 
We are looking into getting a licence for Mold-Design (needed to run the Shrinkage command) in order to do this. The shrinkage for cryo depends on the material that you are using. Some are .98 of the original room temp size, others have a larger differential.


Jason gave me the info on how to warp the part, and it works, but not great. Holes are then seen as just surfaces and dimensioning a diameter cannot be done with the standard diameter dimension (radius has the same issue) and you cannot use the insert command to assemble to holes. Because of those issues, we are looking into the different licence.
 
I think that shrink command is an algorithm that supports shrink in ways more than the simple proportional scale. I would be curious to hear from those Pro/MOLD experts. I've not used it but from what I know about plastic shrink ... that shrink is relative to the nominal wall. When you veer from nominal wall the shrink becomes variable. Any comments?
Edited by: design-engine
 
design-engine said:
I think that shrink command is an algorithm that supports shrink in ways more than the simple proportional scale. I would be curious to hear from those Pro/MOLD experts. I've not used it but from what I know about plastic shrink ... that shrink is relative to the nominal wall. When you veer from nominal wall the shrink becomes variable. Any comments?


I would love to know as well. Right now, I don't agree that we should put this information on the drawing as these are fab drawings and they are not making the parts in a cryo state, they are making them at a particular room temp (it is specified in the overall specs that we reference). The shrunk models that they want on the drawing are only for ref and should not be on the fab drawings (in my mind).
 
I do not believe the shrinkage function actually applies the shrinkage according to wall thickness. I think it is a scaling of the model at the value you set it at. If that is true then you can make a scaled model at the expected shrinkage percentage. or offset the entire surface by a calculated value. It is possible to set the value based on a dimension and specify locations to use custom values:

see here:

shrinkage

However, mold flow and other products should be able to tell you where wall thicknesses would likely produce a sink mark.

This is particularly a problem with plastic gears since the base of the gear tooth is always thicker than the tip.

cheers,

M
 
design-engine said:
I think that shrink command is an algorithm that supports shrink in ways more than the simple proportional scale. I would be curious to hear from those Pro/MOLD experts. I've not used it but from what I know about plastic shrink ... that shrink is relative to the nominal wall. When you veer from nominal wall the shrink becomes variable. Any comments?


Design Engine - shrinkage is not variable is it an absolute factor.


1" with 5% becomes 1.05


.1" with 5% becomes .105.


It is only dependent upon how much volume there is.


Cavities on the part will also increase in size. So, for example, holes in your part would become larger by the increase in shrinkage that you have used.
Edited by: pjw
 
Is it possible to create a UDF with a shrinkage feature in Pro/Mold & then people without Pro/Mold could use it?
 
Don't know if a UDF would work, I don't use them very often. Anyone with the mold package want to try it and let us know?
 
rcamp said:
You could have someone with ProMolddesign a Shrinkage feature in it for you.


We are currently waiting on PTC to get us an evallicense. The paperwork is in their hands, but may be delayed a few weeks as it is quarter end and they are going through the typical big push to make the numbers.
 
Von, I dont think pure shrinkage mentality is really what your interested in. I was faced with a similar issue last year however the Temp diff was in the other direction, working temperature was between 120 deg/c and 140 deg/c. Simple shrinkage is no good here, in the end I used a publish geom feature and modeled in the expansion, this was fine for me as the geomtry was traditional, ie mostly flat machines components or turned components. I didn't go over board and just consider the critical working dims, assembly mating surfaces and areas that had very tight clearance.


If you dont have the license for publish geom you can use a surface copy instead. Because the working part model was a linked child of the fabrication part changes were reflected downstream.


Paddy
 
No UDF, they thought of that:


Can not include shrinkage feature.


You can trick them in with the name game (if you have one in a start file).


or if someone has a file they need it in I can create a shrinkage feature in it and send it back (pay-pal only).


Shrinkage has two formulae as options:


1+S or 1/(1+S)


The difference is insignificant for smaller values.


Once it is created you can redefine it and modifiy it without a ProMold license.


You can shrink some features and not others (based on model tree order shrinks all features that precede it) and shrink X Y Z independently (which can cause cylinders to become non-cylindrical).
 
I could easily send you two parts. Here's how it works:


cast_orig.prt is referenced in cast_merge.prt as a merge feature. After the merge feature there is a shrinkage feature that adds shrinkage to the model. We add all gatinging features to this model and use it to cut our mould. In this way, the original (production) part is unaffected by gate details and we also have the required shrinkage in order to make the mould larger to compensate for shrinkage.


How to use it: Open up your model in session and TEMPORARILY rename it to cast_orig.prt. Be careful if it is a family table member - you will need to do this to the generic. Then open up cast_merge.prt and regenerate. THe merge will pick up YOUR part. Rename your part back to what it should be, rename cast_merge.prt to something sensible and save your work.


Unfortunately, you are unable to add shrinkage feature as a UDF. PTC have prevented this for some unknown reason. I cannot think of such a reason why?


PM me if you would like the files.


Incidentally, you could just use the cast_merge.prt as a template for any new parts you are going to make. You still end up with the shrinkage feature but cuts out the process of having to use a merge.


Phil
Edited by: pjw
 
Phil, I am going to send you a PM with my e-mail address so you can send me a file with the shrinkage feature in there. What version of Wildfire are you on though? I am on WF 3.


Maybe I could send you one of our start parts and you could add the feature and then send it back? I would send either you or rcamp the files we have to add the feature, but I don't know that management would appreciate me doing that!
smiley5.gif
 
I finally got around to playing with the file that Phil sent me. It seems to work (I am going to have the numbers verified by somebody else). We still don't have the license for molding, but it seems we don't need it now...


He sent me a file that uses a merge, shrinkage and model analysis feature. This way, your original file stays the same as it was and you just modify the second file. I think this will work really wel for us as it does everything we wanted!


Thanks much to Phil for sending the file over!
 
Since I had a request for the file, I figured I would host it so others can get to it.


The Pro-e file is here: www.vonhofs.com/files/cast_scaled.prt.1


and I did a write-up on how to use it (we are using Intralink) here: www.vonhofs.com/files/Showing_shrinkage_on_a_part.doc


Remember that you need to decide if you are allowing the part to shrink or grow and you need to choose the proper formula. I needed the parts to shrink so that 1 would be .99851, so I used the 1/1-S formula and used the shrinkage scale of -0.004208 to get it to work properly. Here is the spreadsheet I used to get the number: www.vonhofs.com/files/shrinkage_calcs.xls
 
Glad you finally got what you needed and it looks to be a in a creative way. I don't work with molded parts often but like the technique that Phil used for his parts. I would imagine that being a pretty standard thing to do in his business though.
 

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