I have just started using the hole series for a few things. I had been using
MoldWorks so hadn't needed it much.
I have an assembly with many different configs in it for different plate
thicknesses. When I use the hole series for socket head cap screws, it seems
to work OK. But then when I switch configs, the first thing I notice is that
the holes put in with the hole series are suppressed. Then when I unsuppress
them, I get the following error message: "1/2-13 Tapped Hole1: The intended
hole does not intersect the model."
What's up with that? My other question is if there is a setting someplace
that will apply the hole series holes to all configs??
Thanks for any insight. Is it just that the hole series is incredibly lame
or is it user error???
It's been a long time since I used the hole series myself but IIRC the reason I
quit using it is due to limitations
similar to what you're experiencing. When Cimlogic still owned the product, I
used hole series all the time with no ill
effects. You could put ejector pin holes through all of the mold plates that
were in context to each other. It worked
When SWX bought it, hole series holes quit working the way it used to. Now you
end up with an assembly feature that is
difficult to do anything with. I found that if I changed a plate after a hole
series hole was applied would cause it to
fail and become un-editable. I don't know if any of the problems have been
fixed, but I doubt it.
Yeah, I'm not going to use it anymore. Thanks for the confirmation.
It's kinda funny that SWX is supposedly making this big push to support mold
design with their (currently pretty lame) mold tools. However, if they would
just fix and improve something as seemingly simple as the hole series, they
would be doing a lot more for mold designers than those mold tools ever
reason I quit using it is due to limitations
product, I used hole series all the time with no ill
that were in context to each other. It worked
you end up with an assembly feature that is
hole series hole was applied would cause it to
fixed, but I doubt it.
Well, I did use bad terminology. I didn't mean a true "Assembly Feature".
I was referring to the new hole series icon you get in the assembly FMT.
It looks just like a "cavity feature" icon.
You're welcome to report it Matt. I've grown too complacent over the years.
The configurations in question did indeed have the check-box you are
referring to unchecked which means that the holes should not have been
I use this so seldom that I was initially just looking for confirmation of
how it SHOULD work. You have done that and I will call my VAR as soon as I
hit the send button on this reply. I am lucky to have a great VAR who should
pass this along the appropriate channels. I hadn't reported any bugs all
week. I don't want them to think I'm slacking..........
I tried to send you an e-mail but it failed, so i'll respone to the group
My user name is sparky100 true name [Scott Morley], I wrote a post going
back to 11-7-03 on injection molding. You responded with some good points,
but money is always an issue so we purchased SW. I found it at first hard. I
took a class from SW to get a better understanding of it and it helped a
little. I have also worked on it at home. My boss said up front that it will
not get in the way of getting a projects done. I can understand that because
I know its going to take some time my first time through. My boss asked if I
wanted to try SW on the next job. So, I need to prepare myself. Well, I
would like to know, if you do not mine what kind of molds you design? Bo
Clawson ref. To you on the forum as a full time mold designer with a
boatload of experience. I typically design A-series, stripper-series, and
t-series mold bases. One to two cavity molds. I guess wear to start. I have
not had any time to do mold design at home, just product design. You
responded to my post back on 11-7-03 about Mold Works, Split Works, and Face
Works. Which one works the best. Right now I have no additional software add
to SW, but will be looking into it. I will start out a design from the
beginning. A quick view of how I start a mold frame. I start with an
assembly to make sure all components, side locks, eject pins, core pins,
water, runners, cavity, and core fits without interference from anything. I
need to know, how can I still do it this way. I can not create separate
plates with holes and pockets thinking it going to work. Do I create one
file with all the plates and then do an assembly. Then separate each plate
for detailing after. Please if you could give me any help that would be
great. Also, I do not know how you feel about this, but if you could e-mail
a job that you did form the beginning it might help me out, to study your
feature manger tree with the steps that you did to finish a mold design.
Sorry about the email address. I got to the point of about 300-500
emails a day with all but one being spam, so I shut it down after
notifying people. My good address is below, at least for now.
John Kreutzberger here in the forum is a full time mold designer and
he is the one who mentioned Mold Works & Split Works, etc. I only do
an ocassional mold.
You can use an "Assembly Sketch" to drive the creation of all basic
mold outline and hole features, so that one sketch keeps the base
size, leader pins, ejector pins etc, controlled by one or more
sketches. Search the Solidworks Help for "Assembly Sketch". It makes
a big difference in linking up your solids.
The Solidworks Help is not entirely clear on Assembly Sketch, so here
is a quick outline on how to start any assembly sketch driven set of
1. Open a new "Mold" assembly solids file
2. Create a "Mold PL" sketch on the plane you want to be the parting
3. Put in the mold outline with dimensions and whatever leader pin,
ejector pin holes/points, riser posts, cavity centers & other details
4. Open a new "Aplate" solids file and drop it into the Assembly and
constrain all 3 axes to "Coincident".
5. Open a new "Bplate" solids file and do the same (the common mating
plane of the "Mold PL" assy sketch will be the parting line).
6. Select the "Aplate" in the assembly dwg & choose the Edit
icon/command, add a sketch on the parting line plane and select the
items on the "Mold PL" assembly sketch and use "Convert Entities" to
bring those into the part sketch & extrude the plate solid with or
without holes as you wish.
7. Edit the "Bplate" as in #6.
Now anything you change in the original "Mold PL" sketch in the
assembly solids file will change both the A & B plates.
I do think Solidworks should give some of these simplified outline
procedures, so that it is easier for new users to 'get the jist'.
Good Luck-Have Fun-Create -- Bo