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Thread: Solidworks mold design tools
02-28-2012, 11:20 AM #1Hot Rolled
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- Jan 2006
Solidworks mold design tools
I am designing foundry patterns using solidworks.
Sometimes the mold tool work fairly well for what I need to do, but of course with more complex parts it needs alot of hep.
Is there a book that covers this well? I don't have time right now to take a class.
02-28-2012, 01:57 PM #2
Are you making sand patterns?
how are you aproaching the design?
beause for most of what I would use for foundry or even vacuum form tools I wouldn't use mold tools just regulars modeling, lofting, sweeps, extrudes, revolves, multi-bodies (add-subtract-common), draft, shelling.
injestion molding I use most of the mold tools....but it really depends upon the part.
02-28-2012, 03:36 PM #3Hot Rolled
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- Jan 2006
I have just started using SW on a daily basis, and have to figure this out. I have used ProE in a similar regard but on alot simpiler parts where I just had to copy a couple of surface to pull the cores off. And I have been using Alibre for over a year. With this experience I though that SW would have been a little easier to accomplish this. Maybe I am just going about it backwards.
Yes sand patterns.
Let's say I have a part with a core that goes all the way throught the part. With windows in the middle.
The process that I have been going through:
Create core prints on the model.
Copy/combine to extract cores.(This doesn't work for the model I am working on right now because some of the cored model extends beyond the coreprints.)
Then add stock to represent the insert size to go into my mold boards.
Take off stock accordingly to allow for clearance.
I did try using ruled surface, boundry blends and lofts, but cannot figure out how to use those to extract the core geometry.
How do you go about it.
Maybe I'll have time tonight and make up a quick model so you can help me out.
02-29-2012, 06:46 AM #4
can you put up a pic so I can put it in my minds eye, then I can expand on how I would go about it.
I've done this alot for patterns for RIM Molding using top down assemblies using the cavity tool, make a new part, extrude a blob then use the cavity tool to cut away the pattern shape from the blob. or pic surfaces in the new part from the pattern and offset, then make more surfaces to close the and knit into a solid body again. just some hints.
by the way what part of cheeder you from? I'm originaly from Cedarburg.
02-29-2012, 07:54 AM #5
That wouldnt be TKW Foundry would it? Worked there for a few years, tried to get into the pattern shop but them old buggers just didnt want to retire. Good luck to ya.
02-29-2012, 06:14 PM #6Hot Rolled
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- Jan 2006
What "cavity" tool are you referring too?
Right now I am: Insert, Feature, Copy/move This is to make a disposable part that I can add the prints onto. Then I: Insert, Feature, Combine/subtract to remove excess surfaces.
This seems to work fine it just took a little while to figure out exactly the process to get from point A to point B.
I need to start a more complex pattern tomorrow that I will probably use surfaces to create an offset parting.
I also need to figure out the easiest way to add clearance to the core prints on the pattern. It seems a little backwards to try and offset the surfaces afterwards on more complex prints, but maybe I need to look at making the prints simpler.
Thanks for all the help, today it took about 2-3 hour to get a model to the point where I have it ready to split the pattern and split the core. I did get the core off of the model and created two loose pieces and have the model ready to use the mold tool to make the box model.
It is really interesting doing something that I have done for years on the bench and take that knowledge and relate it to SW. I didn't think it was going to be this hard to figure out, (it seems like some of it could be simplified) but after getting going it shouldn't be too bad.
I am originally from Wisconsin Rapids and am now in Janesville.
I have never worked in a foundry. I took a 2 yr. machine tool class right out of HS and then started at a pattern/mold shop a year latter. The shop I just started at hired is Clinkenbeard and Assoc. in Rockford,IL :
Welcome to Clinkenbeard: Meet Fasterestest!
03-01-2012, 06:19 AM #7
I am curious about the mock-ups your company builds, are they plastic, metal, both, injected, stereolithography, what have you? Pretty cool shit.
03-01-2012, 07:29 AM #8
This was the only way to make molds before they added multi-bodies to SW aka the combine tool and then then mold tools in a part.
You have to do this in an assembly and what is nice you don't loose the part when you subtract like with the combine tool. type in the red header below in the SW help file.
This is something they are now teaching in the mold class your VAR could offer. I used this all the time for model making and for rim mold patterns for a company in Santa Cruz, CA.
If you need help give me a call just PM me and I'll give you my number, you can also see some of my post on SW discussion form: https://forum.solidworks.com/index.jspa
Mold Tools - Cavity
You can create simple molds using the Cavity tool. Creating a mold using the Cavity tool requires the following items:
Design parts - The parts that you want to mold.
A mold base - The part that holds the cavity feature of the design part.
An interim assembly - The assembly in which the cavity is created.
Derived component parts - The parts that become the halves of the mold after you cut them.
You combine the design parts and mold base in the interim assembly. Then, you create a cavity feature in the context of the interim assembly. This relates the mold base to the design part in the event that the design part changes shape.
To create more complex molds, use the tools and techniques presented in Mold Design.
To create a cavity in the mold base:
Insert the design parts and the mold base into an interim assembly.
In the assembly window, select the mold base, and click Edit Component on the Assembly toolbar.
You are editing the part, not the assembly. The changes you make are reflected in the original part file of the mold base. If you do not want to affect the original mold base, use Save As in the mold base part document to save it with a different name for use in each new mold assembly. Otherwise, the original mold base includes the cavity you are about to insert.
Click Cavity on the Mold Tools toolbar, or click Insert, Mold, Cavity.
In the PropertyManager, under Design Components, select the design parts from the FeatureManager design tree.
Under Scale Parameters:
Select the point about which scaling occurs for Scale about.
Component Centroids. Scales the cavity for each part about its own centroid.
Component Origins. Scales the cavity for each part about its own origin.
Mold Base Origin. Scales the cavity for each part about the origin of the mold base part.
Coordinate System. Scales the cavity for each part about the selected coordinate system.
Enter the scaling factor in Scaling %. A positive value expands the cavity, a negative value shrinks the cavity. See Scaling Factor.
Uniform scaling. Select Uniform scaling, and enter a value to scale in all directions.
Non-uniform scaling. Clear Uniform scaling, and enter a scaling value for the X, Y, and Z directions.
Click OK .
A cavity in the shape of the design part is created in the mold base part. The cavity size reflects the scaling factor you specified.
Any changes you make to the design part automatically update the cavity in the mold base, as long as the update path is available. See also External References.
Use the Split tool to separate the mold base part into two pieces.
You cannot edit mold features within an assembly.
03-01-2012, 03:48 PM #9Hot Rolled
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- Jan 2006
Thanks for the help, I am trying to work through the confusion. It looks like the cavity tool is nice, but I still need to figure a couple of things out. Like when I have an upset parting area. I will keep You posted.