Hi,
I'm rather new to the forum, but have used SxWx since the 1997 release. Essentially, I feel that over the last 10 years...I've polished my method of plastic injection mold design using SxWx to where I feel it is one of the fastest (performance-wise) and the least error prone method that I've experienced. I was wondering if any of you mold designers would like to share your thoughts, questions, criticisms, and preferably your own method for designing molds.
The reason for this question, I'm also learning Pro-Enema at my new the job...as that is the main software used here. I see how much better it performs in a lot of areas, and it is making me question whether or not there is a better or faster way to do what I do in SxWx. I personally feel that SxWx can do anything Pro-Enema can do...but faster, easier, and with nicer looking results. I still, however, think that some of the rebuild time’s that I am experiencing could be improved upon…
Before I start, I want to say that I DO NOT use the "mold design" tools that SxWx offers. I was not a fan in the early releases; mainly because the mold-base package simply re-created all the solids...which led to re-detailing all the mold plates any time you so much as moved a screw, etc. In summation, I've only had bad experiences with SxWx mold design tools. Admittedly, it’s been many years since I’ve re-visited the mold design tools.
My method:
1. Part Model:
-Start new part, insert customer model as “base part”, save to XXXX-Product.sldprt
-Apply shrinkage to new part (not altering original customer model)
This seems to cut down on missing references, etc when receiving new customer models during the design process.
2. Cavity/Core Concept Design:
-Start new assembly, insert and locate XXXX-Product.sldprt as needed (bottom of part coincident with “top” plane, etc), and save to XXXX-200(S).sldasm
-Add sketch on front plane, main stack component outlines (cav, core, stripper, etc) and any other splits (gate insert, etc). I fit as much as possible into each.
-Add sketches on side and top planes if necessary (other splits, s/o’s, screw loc’s, dowels, etc)
-Insert new part on origin, save to XXXX-CavBase.sldprt, “edit part” and insert & locate “derived sketch” of all construction sketches on their respective sketch planes then save.
-Open XXXX-CavBase.sldprt and construct main overalls of main cavity block, relating all geometry to the derived sketches.
-Go back into XXXX-200(S).sldasm and while in edit part mode, “cavity” XXXX-Product.sldprt from XXXX-CavBase.sldprt and save all.
-Open XXXX-CavBase.sldprt, and construct any other relevant splits to complete the main parting line (s/o’s, etc), save, and go back into XXXX-200(S).sldasm
-Insert new part on origin, save to XXXX-CoreBase.sldprt, “edit part” and insert & locate “derived sketch” of all construction sketches on their respective sketch planes.
-Create core base part using the derived sketches, with the top of the core extending all the way through the CavBase part.
-Go back into XXXX-200(S).sldasm and edit part (CoreBase)…then “Cavity” the CavBase and Product from the CoreBase part.
2. Cavity/Core Final Design:
-Start new assembly, insert and locate XXXX-200(S).sldasm as needed (plane to plane), and save to XXXX-200.sldasm
-Insert new part on origin, save to XXXX-100.sldprt (main cavity block), “edit part” and insert & locate “derived sketch” of all construction sketches on their respective sketch planes.
-Insert XXXX-CavBase.sldprt into part and fix into position.
-Add any chamfers, rounds, engraving, etc to this model…and also use this model for detailing purposes and final model.
-Repeat above steps for any cavity component touching plastic or otherwise controlled by the construction sketches.
This is getting lengthy, so I will explain how I do the mold base at another time if necessary. It’s essentially the same though; use a sketch assy to drive everything. At the end I have one big top level assembly where I just mate all components in for the assembly drawing and BOM. This way I can just open the construction assemblies for quick changes and updates and not have to load all the unrelated componentry.
Thoughts, questions, comments? I’ve found that the more you limit your “external references”…the faster your assemblies will run. This method makes for only about 4 or 5 external references for each custom part, as all geometry is related to the sketches.
I would appreciate any input that you are willing to offer. Even if you say this method sucks, or you simply have a faster or better way. Ultimately, I’m just looking to use the software to the best of it’s ability. Since I’ve been off of SW for a few years…I wonder if they’ve added any tools that could speed up my process or help w/ performance in any way.
Thanks in advance!
Jeremy Jaeger