CREATING CAVITY IN PRO MOLD 2000i

[al204]

Hello , Im using ProE 2000i. I need to learn how to create a cavity once the model part is ready. I have the Pro Mold/Casting application available. What are the steps that I need to take? I have no manuals or any other literature available to learn on my own.

best regards

Al -
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[dgschaefer]

I think there's a dedicated list at www.ptcuser.org for the mold
package. It's been 6+ years since I worked with it, so I don't think I
could help you much. The basic steps that I remember were to create a
workpiece part that was the same size as the 2 mold halves together,
assemble your design part inside it in a mold assy file, apply shrinkage
to the design part, cut the design part from the workpiece, create
surface quilts to split the workpiece, split and extract the cavity
components and then build the entire mold assy with all your other
components.

Of course, there's a lot to each step, more than you are going to get
from an email list, frankly. Subscribe to the mold list and then dive
in and ask your specific questions there as you have them.

Doug Schaefer

[ptc-726111]

Hi,



Does anyone have an example of a part with knurled features? I need the
knurled features to be modeled in an injection-molded plastic part. The mold
maker will need to build tooling referencing the knurled features, so I am
guessing cosmetic knurling will not be sufficient for this particular
situation. I am creating this part for a third-party, so I do not have
direct contact with this particular injection-molder.



My primarily need is for a SolidWorks file, but I will need to create a
Pro-E as well. As I am concerned about the potential performance hit in
creating a knurled feature that is patterned, I would like to know the best
practices in creating these features (Pro/Engineer and/or SolidWorks) in a
part, especially an injection-molded part with constant wall thickness and
draft angle.





Chris

[cdspk]

The way I produce a knurl is a lefthand and a righthand knurl helical sweep cut then pattern around the axis. Because you need a fast helix, make sure you set the section normal to the trajectory.

Its in the old 'menu manager' functionality which, if you left that behind a while is clunky, but otherwise a pretty simple setup.

[See image attached]

Sean, D&T LU

[ptc-17944]

Check out these links Chris...

http://www.proecentral.com/portal/forum/msgDetail.asp?msg_id=2817&for_id=15

http://www.ptc.com/cs/cs_23/howto/agf362/agf362.htm

Hope they help,

Brad Hacker
Zebra Technologies Corp.

[ptc-726111]

Thanks to everyone who responsed, and sent examples. From the two Pro-E
models sent, the knurled features where modeled as helical cuts, then
patterned (helical cut 1 à pattern, helical cut 2 à pattern). As these
features greatly enlarge the file size, the suggestion of modeling the
datums curves maybe useful one. Placing the physical knurl with its
patterned features maybe best placed as an instance of a family table, which
could be suppressed unless needed.









I don't have a part to show you on, but in the past I have successfully
created knurling on round parts (electrical connectors). Here's what I did:

1. Project a single 45° line on the round part. This wraps the curve around
the part. (i.e. lower left to upper right).

2. Create a sweep cut that follows the projected curve.

3. Pattern the cut. Be VERY careful not to have ANY of the knurl overlap.
(i.e. 80 cuts - pattern 360 / 80 = 4.5°).

4. Project a second single 45° line on the round part in the opposite
direction as the first projected curve. (i.e. lower right to upper left).

5. Follow step 3 again using the second curve.



As you mentioned, this is VERY taxing on the model database. LOT'S of cuts.
Another approach may be to create the first cut as a surface only and then
pattern the surface and then do an EDIT, SOLIDIFY, REMOVE MATERIAL and pick
the surface pattern - or if you are pre-WF, use: CUT, USE QUILT.





Other Pro-E responses:



· The way I produce a knurl is a left-hand and a
right-hand knurl helical sweep cut then pattern around the axis. Because
you need a fast helix, make sure you set the section normal to the
trajectory.

Its in the old 'menu manager' functionality which, if you left that behind a
while is clunky, but otherwise a pretty simple setup.



· In Proe I would use a surface transform, merge the surfaces, and
then cut them away with a surface cut. Surfaces pattern much less memory
intensive than Solid features do, at least in Proe 2001, Wildfire was
suppose to fix these issues but I haven?t come across a really intensive
pattern in a while to test it.