Inventor for Mold App?

[Anonymous]

Hi All,
Just wondering. A parent company of ours is talking about possibly using
inventor for designing molds plastics parts for ventilation systems in hog
barns as well as various cusom plastics.
Just wondering how well inventor works for mold applications and if
anyone has any suggestions before they start digging in?

Thanx Jesse

[Anonymous]

I do injection mold stuff sometimes, mostly consumer products that don't
have conventional shapes. IMWO, IV could use some improvement in that area
but I think they may be working on such improvements (gust a guess). It has
improved a good bit, but I run into cases sometimes where it's not that easy
to get the release angles depending on how the part was made even though I
haven't had one I couldn't get done ... so far anyway. For most applications
I would say it's pretty good and I expect it will get even better.
~Larry

"Jesse" wrote in message
news:7D456089D74A3DEC63A28472DBEAD7A3@in.WebX.maYIadrTaRb...
> Hi All,
> Just wondering. A parent company of ours is talking about possibly
using
> inventor for designing molds plastics parts for ventilation systems in hog
> barns as well as various cusom plastics.
> Just wondering how well inventor works for mold applications and if
> anyone has any suggestions before they start digging in?
>
> Thanx Jesse
>
>

[Anonymous]

Jesse,



We use Inventor considerably (60%) for mold design.



As far as mold base, and or other pure mechanical features (parts) Inventor is fine.



As far as cavity and core geometry, I think there is much room for improvement. In order to get cavity and core geometry straight from the 3D solid (could be an Inventor .ipt, or "step" file, or similar) you must create a derived part. This is the only (practical) way I know to add the shrink factor. (Could be done with proper equations in parameters but would take much work and be error prone... and you may forget to add shrink any particular feature, particullarly if you make changes later... and in this business changes are the order of the day)Once you create the derived part you must now create assemblies (multiple) in which you place the mold component and the derived part. You then must create another derived part that represents the mold by "deriving out" the derived part geometry. Each cavity , core feature will require its own derived component, and maybe its own assembly.



After a while, this starts getting very confusing... keeping tract of the path from part to derived part to multiple assemblies to multiple derived cavity core units.



Also you have to be very careful IF you make changes, as changes, as say to the part, are NOT automatically reflected (updated) through the other derived components. You must go to each of them and make sure thay have updated, and or update them (hit the little lightning bolt). You also must be careful which file you change. For Part changes, you must change the origional part, not the derived part. For mold changes you change the origional mold component IF it does not relate to part geometry, but you must change the derived mold component if the change relates to the mold features derived from the derived part.



Yes... this all sounds very confusing, AND IT IS... too easy to make mistakes, and for $40,000.00, $80,000.00 and so on molds, mistakes are very expensive.



Perhaps the biggest issue with Invemtor is parting lines. If parting lines are complex, varied angles and levels, Inventor simple does not have a way (that I know of) to create the split. For simple, one plane parting lines Inventor works fine. This is biggest drawback.



I hope ADesk works to improve the mold design interface, much like they did for welding, and hope they do it soon. Molding / Mold making is a HUGE market, and a "super" design tool... Inventor "Could" be "it", could be a very profitible one for ADesk.



Just an FYI... several mold shops that I know of use MDT, so that market ADesk already has and can grow as they are weened from MDT to Inventor... BUT, not to happen untill the interface is improved.



Jesse, hope this helps... (and ADesk, hope you have read this as well). I would encourage you to "jump in the water" and give it try. Inventor is a young growing tool, and "down the road" can (should be) the industry leader. Just get familiar with deriving parts, and creating "splits" first.



Regards,



Don A 🙂

[Anonymous]

Even figuring out file names can be a chore xxx-m
xxx-d, yyy-m yyy-d xxx-da... "Now what was it I did to d-sub-a?" ... "I know I
did something, but..." <G>

~Larry

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

"DonA" <djanneken@fuse.net>
wrote in message
href="news:f15b6f1.1@WebX.maYIadrTaRb">news:f15b6f1.1@WebX.maYIadrTaRb...

Jesse,


We use Inventor considerably (60%) for mold design.

As far as
mold base, and or other pure mechanical features (parts) Inventor is fine.


As far as cavity and core geometry, I think there is much room for
improvement. In order to get cavity and core geometry straight from the 3D
solid (could be an Inventor .ipt, or "step" file, or similar) you must create
a derived part. This is the only (practical) way I know to add the shrink
factor. (Could be done with proper equations in parameters but would take much
work and be error prone... and you may forget to add shrink any particular
feature, particullarly if you make changes later... and in this business
changes are the order of the day)Once you create the derived part you must now
create assemblies (multiple) in which you place the mold component and the
derived part. You then must create another derived part that represents the
mold by "deriving out" the derived part geometry. Each cavity , core feature
will require its own derived component, and maybe its own assembly.


After a while, this starts getting very confusing... keeping tract of
the path from part to derived part to multiple assemblies to multiple derived
cavity core units.

Also you have to be very careful IF you make
changes, as changes, as say to the part, are NOT automatically reflected
(updated) through the other derived components. You must go to each of them
and make sure thay have updated, and or update them (hit the little lightning
bolt). You also must be careful which file you change. For Part changes, you
must change the origional part, not the derived part. For mold changes you
change the origional mold component IF it does not relate to part geometry,
but you must change the derived mold component if the change relates to the
mold features derived from the derived part.

Yes... this all sounds
very confusing, AND IT IS... too easy to make mistakes, and for $40,000.00,
$80,000.00 and so on molds, mistakes are very expensive.

Perhaps the
biggest issue with Invemtor is parting lines. If parting lines are complex,
varied angles and levels, Inventor simple does not have a way (that I know of)
to create the split. For simple, one plane parting lines Inventor works fine.
This is biggest drawback.

I hope ADesk works to improve the mold
design interface, much like they did for welding, and hope they do it soon.
Molding / Mold making is a HUGE market, and a "super" design tool... Inventor
"Could" be "it", could be a very profitible one for ADesk.

Just an
FYI... several mold shops that I know of use MDT, so that market ADesk already
has and can grow as they are weened from MDT to Inventor... BUT, not to happen
untill the interface is improved.

Jesse, hope this helps... (and
ADesk, hope you have read this as well). I would encourage you to "jump in the
water" and give it try. Inventor is a young growing tool, and "down the road"
can (should be) the industry leader. Just get familiar with deriving parts,
and creating "splits" first.

Regards,

Don A
:-)

[Anonymous]

Jesse,

Go to www.seamech.com and check Products > Composites for some examples of
vacuum formed parts done in Inventor. They make air condition units for
private airplanes.
--
Regards,
John

"Jesse" wrote in message
news:7D456089D74A3DEC63A28472DBEAD7A3@in.WebX.maYIadrTaRb...
> Hi All,
> Just wondering. A parent company of ours is talking about possibly
using
> inventor for designing molds plastics parts for ventilation systems in hog
> barns as well as various cusom plastics.
> Just wondering how well inventor works for mold applications and if
> anyone has any suggestions before they start digging in?
>
> Thanx Jesse
>
>

[Anonymous]

AFAIK, the following statement is not quite
accurate. If you have a set of files that are associatively related to each
other through assemblies or derived components, you should be able to update all
the files by updating _one_ assembly or derived assembly file that depends on
all the other files (This is especially true if there is no adaptivity among the
files).

Updating is supposed to work regardless of the
"depth" of the file dependency "structure." If you have any example where things
are not updating properly I would ask you to please submit a bug
report.

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

"DonA" <djanneken@fuse.net>
wrote in message
href="news:f15b6f1.1@WebX.maYIadrTaRb">news:f15b6f1.1@WebX.maYIadrTaRb...

Also
you have to be very careful IF you make changes, as changes, as say to the
part, are NOT automatically reflected (updated) through the other derived
components. You must go to each of them and make sure thay have updated, and
or update them (hit the little lightning bolt).

[Anonymous]

Well put Don A. Especially in regards to irregular part lines. If
inventor wants to keep up, an improvement here is a must.
--
Billy Hiebert
HIEBERT SCULPTURE WORKS
Small Part Injection Molding
http://www.hieberts.com

DonA wrote:

> Jesse,
>
> We use Inventor considerably (60%) for mold design.
>
> As far as mold base, and or other pure mechanical features (parts)
> Inventor is fine.
>
> As far as cavity and core geometry, I think there is much room for
> improvement. In order to get cavity and core geometry straight from the
> 3D solid (could be an Inventor .ipt, or "step" file, or similar) you
> must create a derived part. This is the only (practical) way I know to
> add the shrink factor. (Could be done with proper equations in
> parameters but would take much work and be error prone... and you may
> forget to add shrink any particular feature, particullarly if you make
> changes later... and in this business changes are the order of the
> day)Once you create the derived part you must now create assemblies
> (multiple) in which you place the mold component and the derived part.
> You then must create another derived part that represents the mold by
> "deriving out" the derived part geometry. Each cavity , core feature
> will require its own derived component, and maybe its own assembly.
>
> After a while, this starts getting very confusing... keeping tract of
> the path from part to derived part to multiple assemblies to multiple
> derived cavity core units.
>
> Also you have to be very careful IF you make changes, as changes, as say
> to the part, are NOT automatically reflected (updated) through the other
> derived components. You must go to each of them and make sure thay have
> updated, and or update them (hit the little lightning bolt). You also
> must be careful which file you change. For Part changes, you must change
> the origional part, not the derived part. For mold changes you change
> the origional mold component IF it does not relate to part geometry, but
> you must change the derived mold component if the change relates to the
> mold features derived from the derived part.
>
> Yes... this all sounds very confusing, AND IT IS... too easy to make
> mistakes, and for $40,000.00, $80,000.00 and so on molds, mistakes are
> very expensive.
>
> Perhaps the biggest issue with Invemtor is parting lines. If parting
> lines are complex, varied angles and levels, Inventor simple does not
> have a way (that I know of) to create the split. For simple, one plane
> parting lines Inventor works fine. This is biggest drawback.
>
> I hope ADesk works to improve the mold design interface, much like they
> did for welding, and hope they do it soon. Molding / Mold making is a
> HUGE market, and a "super" design tool... Inventor "Could" be "it",
> could be a very profitible one for ADesk.
>
> Just an FYI... several mold shops that I know of use MDT, so that market
> ADesk already has and can grow as they are weened from MDT to
> Inventor... BUT, not to happen untill the interface is improved.
>
> Jesse, hope this helps... (and ADesk, hope you have read this as well).
> I would encourage you to "jump in the water" and give it try. Inventor
> is a young growing tool, and "down the road" can (should be) the
> industry leader. Just get familiar with deriving parts, and creating
> "splits" first.
>
> Regards,
>
> Don A 🙂

[Anonymous]

I was at NDES this year and AutoDesk was showing
their new core and cavity package that is supposed to be coming out this
summer.  I didn't get a good look at it, but it looks like AutoDesk is
trying to make some headway into this market.

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

"DonA" <djanneken@fuse.net>
wrote in message
href="news:f15b6f1.1@WebX.maYIadrTaRb">news:f15b6f1.1@WebX.maYIadrTaRb...

Jesse,


We use Inventor considerably (60%) for mold design.

As far as
mold base, and or other pure mechanical features (parts) Inventor is fine.


As far as cavity and core geometry, I think there is much room for
improvement. In order to get cavity and core geometry straight from the 3D
solid (could be an Inventor .ipt, or "step" file, or similar) you must create
a derived part. This is the only (practical) way I know to add the shrink
factor. (Could be done with proper equations in parameters but would take much
work and be error prone... and you may forget to add shrink any particular
feature, particullarly if you make changes later... and in this business
changes are the order of the day)Once you create the derived part you must now
create assemblies (multiple) in which you place the mold component and the
derived part. You then must create another derived part that represents the
mold by "deriving out" the derived part geometry. Each cavity , core feature
will require its own derived component, and maybe its own assembly.


After a while, this starts getting very confusing... keeping tract of
the path from part to derived part to multiple assemblies to multiple derived
cavity core units.

Also you have to be very careful IF you make
changes, as changes, as say to the part, are NOT automatically reflected
(updated) through the other derived components. You must go to each of them
and make sure thay have updated, and or update them (hit the little lightning
bolt). You also must be careful which file you change. For Part changes, you
must change the origional part, not the derived part. For mold changes you
change the origional mold component IF it does not relate to part geometry,
but you must change the derived mold component if the change relates to the
mold features derived from the derived part.

Yes... this all sounds
very confusing, AND IT IS... too easy to make mistakes, and for $40,000.00,
$80,000.00 and so on molds, mistakes are very expensive.

Perhaps the
biggest issue with Invemtor is parting lines. If parting lines are complex,
varied angles and levels, Inventor simple does not have a way (that I know of)
to create the split. For simple, one plane parting lines Inventor works fine.
This is biggest drawback.

I hope ADesk works to improve the mold
design interface, much like they did for welding, and hope they do it soon.
Molding / Mold making is a HUGE market, and a "super" design tool... Inventor
"Could" be "it", could be a very profitible one for ADesk.

Just an
FYI... several mold shops that I know of use MDT, so that market ADesk already
has and can grow as they are weened from MDT to Inventor... BUT, not to happen
untill the interface is improved.

Jesse, hope this helps... (and
ADesk, hope you have read this as well). I would encourage you to "jump in the
water" and give it try. Inventor is a young growing tool, and "down the road"
can (should be) the industry leader. Just get familiar with deriving parts,
and creating "splits" first.

Regards,

Don A
:-)

[Anonymous]

Adesk,



I have tried association as well. BUT, I have never (yet) been able to get a .idw to update "automatically" when changing lets say the "origional" part.



Lets take a detailed look at my process and perhaps you can explain where I go wrong and or need improvements and or changes... My OBJECTIVE is to create a paper drawing of a mold cavity, which I will call mold-block1.



I start with... "part.ipt"



I then create "derived-part.ipt"



I then create "mold-block1.ipt"



I then create "assembly-1.iam" which consists of "mold-block.ipt" and "derived-part.ipt"



I then create "derived-mold-block1.ipt" from "assembly-1.iam". I create the "derived-mold-block1.ipt by deriving out the "derived-part.ipt" portion.



I then create "mold-drawing.idw".



I then place a view of "derived-mold-block1.ipt into the "mold-drawing.idw"



FINALLY... I now have a detailed drawing of derived-mold-block1.ipt which is my origional objective (mold-block1). FINE... no problem, other than its confusing as he _ _. Now the BIG BUT... I make a change to the origional "part.ipt". What I would "expect" is that after I update the "part.ipt" file that the view of "derived-mold-block1.ipt, within the "mold-drawing.idw" file would be automatically updated. BUT IT's NOT.



What I have been doing is to go to the "derived-part.ipt" and hit lightning bolt, then go to the "assembly-1.iam" and hit lightning bolt, then go to "derived-mold-block" and hit lightning bolt, then go to the "mold-drawing.idw" and it will then update.



Heaven help me if I forget one of the updates along the way.



Now... this is just for one mold component. Molds may consist of several... 10, 30, perhaps more components. Try to keep this process straight for that many files, and you will be as insane as I am getting.



So ADesk... PLEASE make this process MUCH MUCH more simple.



And... while your at it please improve upon parting lines.



Thank You and Regards



Don A 🙂



PS sorry about this extra long reply, if I could make the process (create "mold-block1") simpler then the post would be proportional.

[Anonymous]

Joe,



Sounds great to me... can't be too soon.



Just wondering though... with V7 just released (April), and summer is just around the corner, will ADesk have an upgrade mold package for V7? Or will there be a V8 that includes a mold package? Or will there not be a mold package relaese anytime soon? My guess is the later, buy hopeing for the earlier.



Thanks for the info.



Regards,
Don A 🙂

[Anonymous]

Don,

There is an issue that drawings do not allow you to
update all the files when one file changes. But all part and assembly files will
allow get updated when the "top most" file is updated.

In your example,
size=3>derived-mold-block1.ipt contains three part
files and one assembly file "under" it. If any of these four files were to
change you can get everything to update properly by updating only
face="Times New Roman" size=3>the derived-mold-block1.ipt
.

Let's say that you have a large number of component
like derived-mold-block1.ipt,
all dependent on part.ipt, that you want to update conveniently. Just create a
"dummy" assembly and place all these components in that (you don't need to
bother to position or constrain them). Now if you were to change part.ipt (or
any other part or assembly anywhere), just update the dummy assembly, and
everything should update properly (note that the dummy assembly is the top most
part/assembly).

HTH.

PS: you are absolutely right about the limitations
with parting lines and parting surfaces.

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

"DonA" <djanneken@fuse.net>
wrote in message
href="news:f15b6f1.7@WebX.maYIadrTaRb">news:f15b6f1.7@WebX.maYIadrTaRb...

Adesk,


I have tried association as well. BUT, I have never (yet) been able to
get a .idw to update "automatically" when changing lets say the "origional"
part.

Lets take a detailed look at my process and perhaps you can
explain where I go wrong and or need improvements and or changes... My
OBJECTIVE is to create a paper drawing of a mold cavity, which I will call
mold-block1.

I start with... "part.ipt"

I then create
"derived-part.ipt"

I then create "mold-block1.ipt"

I then
create "assembly-1.iam" which consists of "mold-block.ipt" and
"derived-part.ipt"

I then create "derived-mold-block1.ipt" from
"assembly-1.iam". I create the "derived-mold-block1.ipt by deriving out the
"derived-part.ipt" portion.

I then create "mold-drawing.idw".


I then place a view of "derived-mold-block1.ipt into the
"mold-drawing.idw"

FINALLY... I now have a detailed drawing of
derived-mold-block1.ipt which is my origional objective (mold-block1). FINE...
no problem, other than its confusing as he _ _. Now the BIG BUT... I make a
change to the origional "part.ipt". What I would "expect" is that after I
update the "part.ipt" file that the view of "derived-mold-block1.ipt, within
the "mold-drawing.idw" file would be automatically updated. BUT IT's NOT.


What I have been doing is to go to the "derived-part.ipt" and hit
lightning bolt, then go to the "assembly-1.iam" and hit lightning bolt, then
go to "derived-mold-block" and hit lightning bolt, then go to the
"mold-drawing.idw" and it will then update.

Heaven help me if I forget
one of the updates along the way.

Now... this is just for one mold
component. Molds may consist of several... 10, 30, perhaps more components.
Try to keep this process straight for that many files, and you will be as
insane as I am getting.

So ADesk... PLEASE make this process MUCH MUCH
more simple.

And... while your at it please improve upon parting
lines.


Thank You and Regards

Don A 🙂

PS sorry
about this extra long reply, if I could make the process (create
"mold-block1") simpler then the post would be
proportional.

[Anonymous]

Adesk,



Thanks for the feedback. Sounds like this method (dummy assembly) will simplify things considerably.



If I understand correctly, after making changes to any of the .ipt's, with the assumption that they are all in the dummy assembly, then all I need to be concerned with is updating the dummy assembly.



However, once the dummy assembly is updated I will have to go to (open and or access) the drawing (.idw) and it should then update.



If this is correct, then I see this as no major issue. The fact that I have to remember to update only two files (.iam & .idw) is not hard to remember.



I will be trying this soon to see how it works. Again thanks for the reply... it is GREATLY APPRECIATED.



In the meantime... I will be anxiously waiting for ADesk to "create" and efficient ('more') "mold interface" within Inventor.



Regards,



Don A 🙂

[Anonymous]

ADesk,



:-)))))))))))



Tried it... works GREAT. MUCH THANKS.



Regards,



Don A 🙂