Tutorial: SolidWorks Mold Tools
This Tutorial was written "Barney Style" so even the most novice of SolidWorks users should be able to follow easily.
The files I created making this tutorial can be found here:
Tutorial: SolidWorks Mold Tools
Open up SolidWorks.
To turn on the tool bar with the mold tools we will be using in this tutorial, right click in blank portion of the tool bar and this will open the "CommandManagers" - about half way down you find an icon labeled "MoldTools".
Click this and it will add the mold tools toolbar to your window and this can be moved wherever you find convenient.
Start a new part
This part is made in centimeters.
click on the options button then then select the Document Properties tab. from here select units and click the CGS bullet.
When finished select OK button on the bottom.
Create a plane offset from the top plane by 15cm
here is our new plane
open a new sketch on this new plane.
(you can right click the plane in the feature tree and select the sketch icon to do this)
Create the following sketch then exit the sketch.
With the sketch we just created selected, press the extruded boss/base button in the features menu.
Extrude down 15 cm with 6 degrees of draft angle
Now We will use the shell comand
Select the top face and make the wall thickness 0.5 cm.
Now that we have the basic basket, it needs a rim. open a sketch on our plane 1 again.
use the convert entities button
Select the segments that make up the inner loop of the top edge of the basket. and press green check mark to accept.
now use offset Entities.
select the same inside loop from before and offset it 1.5 cm
exit this sketch
With the last sketch still selected, choose the extruded boss/base button from the features menu ribbon.
extrude down .5 cm.
Now to make the cuts in the side of the basket we will start with opening a sketch on the right plane.
Hit the space-bar and this will bring up a window to change the view. Lets make it normal to our sketch plane.
Draw the sketch shown and then exit out of the sketch.
Now in the features ribbon we will use the extruded cut option.
Set directions 1 and 2 to through all.
Now to pattern the cut, use the linear pattern tool.
For Direction 1, choose the vertical edge highlighted in orange.
Set the spacing to 6 cm and the number of instances to 2.
Accept the settings by clicking the green check.
Now for a few fillets
add .5 cm fillets to the inside top and bottom edges.
Now that our part is done, we need to perform Draft Analysis on it before we can start making our mold.
After clicking on the draft analysis icon, we need to select the top plane as the direction of pull and a draft angle of 1 degrees and then press the green check.
The faces of our part will change color depending on the draft of the face. We can see the edge around the top lip of our basket is yellow and needs draft added to it.
Clicking the green check again will exit out of draft analysis.
To add the required draft, we will right click on the feature needing it (boss-extrude2) and click the upper left icon allowing us to edit this feature.
click the draft icon and this will draft the feature.
Now when we perform our draft analysis we can see that face is no longer yellow and is now red.
Our part is almost ready to make a mold now.
Depending on the material, the part will shrink when cooled after molding. Therefor our mold needs to be a little larger then we want our final part to be. So we will scale up our part.
Click the scale button in mold tools menu.
For this model we will scale it uniformly about the centroid with a scale factor of 1.02 but you can play around with the options to see what will happen.
Now to make a parting line.
The parting line will separate the positive and negatively drafted faces (the red from the green when we did the draft analysis) and this is also where the two halves of our mold will meet.
Click the Parting Line icon.
Select the top face of the basket to define the direction of pull for our mold and set the draft angle to 1 degree.
Also be sure that the box for "use for core/cavity is checked.
Then click the draft analysis button.
the parting line is created at the intersection of the positive and negatively drafted faces (red and green).
click the green check and our parting line is created.
Now to create shut-off surfaces. We need these because of the cutout holes in the side of the basket. These surfaces will denote where the core and cavity halves of the mold will meet.
Click on the shut-off surfaces icon.
The openings in the part are automatically detected and the inner edge of each opening is automatically selected.
Be sure the knit option is selected.
In the reset all patch types menu, click the all tangent button (the right one with a cross in the ball).
after clicking the green check, you will see in the feature tree that you now have both solid bodies and surface bodies.
You can hide the solid body and expand the surface bodies menu and hide any of the surface bodies to see what you have.
Here are the cavity and core surface bodies with the solid body of the part hidden...
just the cavity surface...
just the core surface...
and just the solid body of the part.
(notice that part is encased between the two surfaces)
Now we need to create a parting surface. This surface extends away from the part and is the surface that separates the two halves of the mold from each other.
Click on the Parting Surfaces icon.
for this mold we will use the mold parameter of perpendicular to pull and the parting line will automatically be selected.
Make sure the rest of the settings are as shown in the picture and then click the green check to complete.
Now that we have these three surfaces it is time to create the mold.
First we need to create a plane that will be where our two halves of the mold meet.
create a plane that is offset 2 cm above the top of our part.
with this new plane still selected, click the tooling split icon.
This will open a new sketch on that plane. Draw the sketch shown in the picture.
When you exit the sketch, it will bring you to the tooling split Property Manager.
select the interlock surface box. this allows the two halve to the mold to interlock with each other allowing for them to stay properly aligned.
Set the other dimensions as shown in the picture.
It already knows what are surfaces are and has them properly selected.
click the green check and our mold is created.
if you look at the feature tree, you can see that now we have three surface bodies and three solid bodies.
take some time to hide these to see what we have.
Here is the cavity and the part. As you can see, the part will be stuck in the cavity because of the cutouts in the basket.
just the cavity...
and the core...
and our basket...
Now lets make sure everything is hidden except for our basket so we can perform undercut analysis on it.
Click the undercut analysis icon.
The direction of pull is already decided and we just have to click the green check.
like in the draft analysis, different faces become color coded. The red faces are the ones we need to create side cores to mold.
Click the check or x to exit the undercut analysis colors and exit.
To create the cores for the basket cutouts, click the core icon.
Select the outer face of the basket with the cuts in it.
This will open a sketch. I find it easier to sketch with normal to the sketch plane.
create this sketch.
When you exit the sketch, the core property manager will appear.
change the core/cavity body to tooling split one
in the direction field select a line in direction of pull of the core.
select though all for direction 1 and un-check the cap ends box.
when you click the green check your core will be created.
Now repeat steps 65 to 72 and reference this picture to create the core on the other side.
(some of the direction will be goofy if you try to do it exactly as done in 65 - 72 so look at the settings below.)
Here is the completed mold parts.
I moved the individual solid bodies apart like an exploded view so you can see the different parts.
A different angle
Here is some of the great FREE stuff sent to me from www.protolabs.com