AnsweredAssumed Answered

Meaning of Negative & Positive Draft Angles in Molds?

Question asked by Daniel Sevier on Oct 31, 2018
Latest reply on Nov 6, 2018 by Daniel Sevier

Like • Show 0 Likes0
Comment • 12

I am new to mold making, and I am trying to figure out what is meant by Negative vs. Positive draft angles.

I understand that the part needs to be drafted to more easily pop out of the mold. I found this explanation from Solidworks:

2010 SOLIDWORKS Help - Draft Analysis Overview

From this site, I understand that defining a part's face as having a positive or negative draft is based upon the reference angle, but I really don't understand what this reference angle is in "reference" to. My guess is the pull direction somehow, but don't understand why the upper cope of the mold wouldn't just be pulled straight up at a 0 deg reference angle (if this is what that means).

I created a part file to create an example and attached it here. I just picked the front plane as the reference split plane, and the pull direction is normal to this. I am just using the default green, yellow, red color-coding for Draft Evaluation.

In the part, the angles are all 15 degrees, and the flat sides have no draft. If someone could please explain to be the actual meaning behind the relationship between the positive and negative part angles and the reference angle, I'd appreciate it.

I think I am partially confused because other sites have images such as these:

Thank you!!

Doug Seibel Nov 6, 2018 8:48 AM

Correct Answer

Daniel Sevier wrote:

Thanks all for your helpful input.
I guess I still have some confusion, so I have some put some images here to consider:

So, this is the "reference angle" to which I was referring:

I'd like to understand this reference angle relative to the reference split plane and relative to the part's facial draft angles.

You can see in my example model (with 15 degree drafts on faces) that as soon as 15 degrees is exceeded in the reference angle, then the face turns yellow (from green with a positive draft), indicating that it needs more draft. I'm finding it difficult to visualize why this would be a problem. (You can see I just input 15.01 degrees as the reference angle to test this.)

So, if the orange angle is the reference angle and is greater than the facial draft angle, how would the parts get stuck? (or do I have it drawn wrong?) Thanks for your help!!

The "Reference angle" is nothing more than a value that YOU set.

Let's say, for instance, that I am tasked with designing a mold for this part...

And when I go over the finish requirement for this part, I learn that they are wanting to have a specific "leather" texture on all the "show" (visible by the end user / customer) surfaces. I quickly check and find that the minimum draft required for that specific texture is 6 degrees. So I launch the Draft Analysis tool, select the proper reference plane, and enter 6 degrees for the reference angle. Now, any area of the part that has less than 6 degrees draft, Solidworks will color yellow.

As we can clearly see...the part, as currently designed, has areas that do not have enough draft for the desired texture.

(One thing that is important to note regarding the "Reference Angle" in relation to the "Reference Plane"...Zero degrees is perpendicular to the Reference Plane, NOT parallel.)

So now I can quickly go back to the customer and show them that their part does not have enough draft for the texture they had originally desired. At this point, they could choose to change the part model to allow for the desired texture, or they could change the texture specification to accommodate the existing part design.

The "Reference Angle" can be any value you desire/require.

See the reply in context

Attachments

draft test.SLDPRT.zip53.2 KB

No one else had this question

Outcomes

Deepak Gupta Nov 4, 2018 3:59 AM

In my understanding the draft (i.e. negative or positive) in the mold making is based on the direction of the pull. And the reference is taken based on the parting line/surface (where core and cavity meet).

If a part has enough draft and it can pulled out of the core or cavity then that draft is called positive draft like in the picture below where red color indicates the molded component and arrow defines the direction from where part would come out from cavity. Since the part won't stuck during the pull out process, the draft is the positive draft.

Now for the below picture; the part won't come out and get trapped in the cavity, so the draft is the negative draft.

The draft angle can varies on material, length/depth of the part, wall thickness, etc. And it is always recommended to have some draft on the walls else the walls would rub against the core and cavity which would damage the mold.

Now depending on your mold design the pull direction and draft would be decided i.e. positive or negative.

Here is a simple mold where green indicated cavity, red indicates core and blue indicate the part.

When mold would open the part would move along with cavity or core depending on the design, mold type and requirements. Let's assume it would move with cavity.

So in this case the pull direction is downwards (because core is pulled away from the part), hence draft angle is positive (shown by green color on the cavity in picture below).

In a mold you may need both positive and negative draft depending on the part design. Both sides may not be positive or negative as the part would get trapped into the mold. Based on your test model, both negative and positive draft are needed and software would indicate bottom one side as positive and other side as negative based on the pull direction.

I hope this doesn't add more confusion and help to some extent.

Actions

Snehal Shah Nov 4, 2018 7:11 AM

Daniel you must be aware that draft is a taper given in vertical faces w.r.t. parting line for easy withdrawal of die/pattern from mould.

These are basic foundry shop terminologies.

There are 3 types of draft.

1. Negative draft

2. Positive draft

3. Positive-Negative draft

1. Negative draft reduces basic dimension within permissible tolerances. (refer ISO 8062).

2. Positive draft adds to basic dimension, which can be removed later on by machining or grinding process.

3. Positive-Negative draft is a combination of both types. Where height dimn. is much more after parting the job; giving it -ve draft will result in heavy reduction in material at top or giving it +ve draft will result in heavy extra material at parting line. To compensate this +ve-ve draft is given.

Reference angle is nothing but draft angle w.r.t. parting line.

Hope this helps.

If you still have any questions regarding foundry/castings/moulds....just knock-knock.

regards,

Snehal

Attachments

DRAFT IN MOULD.SLDPRT.zip113.0 KB

Actions

Ruben Balderrama Nov 5, 2018 8:25 AM

Buy a book

Gastrow Injection Molds: 130 Proven Designs: Amazon.es: Peter Unger: Libros en idiomas extranjeros

You can design a product with negative and positive draft angles.

Wich is the difference? Cost/Money/Cheaper.

You on design has some restriction like that, on construction you don't have restriction, because you need to make it able....

Actions

Doug Seibel Nov 5, 2018 9:13 AM

Reference Plane:

Movement of the mold/action will be perpendicular to this plane. It is also commonly called the "Pull Plane". The "direction" is normally set so that the arrow is pointing to the cavity-side of the mold or, in the case of side-pull action, the direction of retraction.

Positive Draft:

Often referred to as "Cavity-side" draft.

Negative Draft:

Often referred to as "Core-side" draft.

Molded parts must have draft. Faces/surfaces that are perfectly vertical from the reference plane are something that is exceeding undesirable. Everything needs draft...some things need more draft than others.

For instance, take a look at all the plastic in your vehicle...the dash, the steering wheel, the door panels, the glove box, and so many other things...do you notice how many of them have some type of "texture" to them? Some have a texture to make them look a bit like leather, some have a smooth but dull or matte satin finish...every single plastic item that you see has some type of intentional texture on it. Different textures require different minimum angles to release from the mold without the mold causing damage to the texture molded onto the plastic part.

Another critical draft is where there are "jogs", "jumps", or "transitions" in the parting line surfaces. Angles of 3 degrees or less are what is known as "self-locking" angles, and need to be avoided.

Self-Locking Angles/Tapers: Angles of less than 3 degrees per side. Some use the "rule of thumb" of 7 degrees included angle, or 3.5 degrees per side. If you grind a tapered pin with 2 degrees per side draft on the diameter, and put it into a mating hole that has the same draft, it will "lock" into the hole. It will take significantly greater force to remove the pin, than was used to install it. This condition is extremely undesirable/destructive on a mold. Conversely, there are Self-Releasing Angles/Tapers...which are simply angles greater than what would be a Self-Locking Angle/Taper. Grind a tapered pin with a 5 degree per side draft on the diameter and put it into a mating hole that has the same draft, and the pin will fall out of the hole if you turn it upside down and let it fall out...beat on it with a hammer and turn it upside down and it will still fall out freely. Self-Locking Angles are very bad in a mold, Self-Releasing Angles are very good.

The draft analysis tool in Solidworks help you identify whether or not the part is drafted properly for being molded.

FYI...

The default Green/Yellow/Red coloring setup is, imho, very limited in is usefulness. I recommend changing the Red to Blue, so that it will be more useful when you click on "Gradual transition". Only use the "three color" draft analysis for making sure textured surfaces have enough draft and parting line jogs have enough draft. The "Gradual transition" allows you to better see everything else (like back-draft, undercuts, zero draft, etc.).

Actions

Steven McCallion Nov 5, 2018 9:35 AM

This is one of those things like word mispellings that I've just given up on in my life, because no matter how much effort I put into trying to remember it I just end up forgetting it anyway the next week; trying to remember if separate is seperate vs separate for example. Thus when I use the draft tool I set the draft to a big number where I can see clearly on the screen that it's drafting in the correct direction, and then adjust appropriately.

Such a rebel.

Actions

Daniel Sevier Nov 5, 2018 1:25 PM

Thanks all for your helpful input.

I guess I still have some confusion, so I have some put some images here to consider:

So, this is the "reference angle" to which I was referring:

I'd like to understand this reference angle relative to the reference split plane and relative to the part's facial draft angles.

You can see in my example model (with 15 degree drafts on faces) that as soon as 15 degrees is exceeded in the reference angle, then the face turns yellow (from green with a positive draft), indicating that it needs more draft. I'm finding it difficult to visualize why this would be a problem. (You can see I just input 15.01 degrees as the reference angle to test this.)

So, if the orange angle is the reference angle and is greater than the facial draft angle, how would the parts get stuck? (or do I have it drawn wrong?) Thanks for your help!!

Actions

Deepak Gupta @ Daniel Sevier on Nov 5, 2018 1:57 PM

Please do not get mixed up with the draft analysis and mold. Draft analysis is a way to find any faces with less draft (means small angle value vs the specified value; so 15 vs 15.01 in your case), faces with no drafts or faces with draft in reversed direction (positive or negative draft) instead of in correct direction (in simple words, face have negative draft when positive was required on that face or face have positive draft when negative was required on that face).

Now since required draft is 15.01 (as you've specified), the draft analysis tool is indicating the faces (using yellow color and marking them under required draft) that have less draft angle than the specified value

Based on the following picture, you've drawn the reference angle correctly. The part won't get stuck in the mold since it already has some draft but molded part dimensions may not be correct since the reference angle (required draft value, 15.01 in this case) is not same as on the part (given drat value, 15 in this case).

Actions

Daniel Sevier @ Deepak Gupta on Nov 6, 2018 10:45 AM

Thanks Deepak! Makes much more sense now!

Actions

Doug Seibel @ Daniel Sevier on Nov 6, 2018 8:48 AM

Daniel Sevier wrote:

Thanks all for your helpful input.
I guess I still have some confusion, so I have some put some images here to consider:

So, this is the "reference angle" to which I was referring:

I'd like to understand this reference angle relative to the reference split plane and relative to the part's facial draft angles.

You can see in my example model (with 15 degree drafts on faces) that as soon as 15 degrees is exceeded in the reference angle, then the face turns yellow (from green with a positive draft), indicating that it needs more draft. I'm finding it difficult to visualize why this would be a problem. (You can see I just input 15.01 degrees as the reference angle to test this.)

So, if the orange angle is the reference angle and is greater than the facial draft angle, how would the parts get stuck? (or do I have it drawn wrong?) Thanks for your help!!

The "Reference angle" is nothing more than a value that YOU set.

Let's say, for instance, that I am tasked with designing a mold for this part...

As we can clearly see...the part, as currently designed, has areas that do not have enough draft for the desired texture.

(One thing that is important to note regarding the "Reference Angle" in relation to the "Reference Plane"...Zero degrees is perpendicular to the Reference Plane, NOT parallel.)

The "Reference Angle" can be any value you desire/require.

Actions

Daniel Sevier @ Doug Seibel on Nov 6, 2018 10:45 AM

Thanks! Makes much more sense now with the clarification about the reference angle being what I choose to set.

Actions

12 Replies

ömür tokman Nov 3, 2018 10:03 AM
Mark Correct
Correct Answer
Hi Daniel
Reference is the point of separation of the mold.
https://www.youtube.com/watch?v=M95bhPrDwA0

https://www.youtube.com/watch?v=IYZOTt9zTv0
https://www.youtube.com/watch?v=b1U9W4iNDiQ
Like • Show 2 Likes2
Actions
Deepak Gupta Nov 4, 2018 3:59 AM
Mark Correct
Correct Answer
In my understanding the draft (i.e. negative or positive) in the mold making is based on the direction of the pull. And the reference is taken based on the parting line/surface (where core and cavity meet).

If a part has enough draft and it can pulled out of the core or cavity then that draft is called positive draft like in the picture below where red color indicates the molded component and arrow defines the direction from where part would come out from cavity. Since the part won't stuck during the pull out process, the draft is the positive draft.

Now for the below picture; the part won't come out and get trapped in the cavity, so the draft is the negative draft.

The draft angle can varies on material, length/depth of the part, wall thickness, etc. And it is always recommended to have some draft on the walls else the walls would rub against the core and cavity which would damage the mold.

Now depending on your mold design the pull direction and draft would be decided i.e. positive or negative.

Here is a simple mold where green indicated cavity, red indicates core and blue indicate the part.

When mold would open the part would move along with cavity or core depending on the design, mold type and requirements. Let's assume it would move with cavity.

So in this case the pull direction is downwards (because core is pulled away from the part), hence draft angle is positive (shown by green color on the cavity in picture below).

In a mold you may need both positive and negative draft depending on the part design. Both sides may not be positive or negative as the part would get trapped into the mold. Based on your test model, both negative and positive draft are needed and software would indicate bottom one side as positive and other side as negative based on the pull direction.

I hope this doesn't add more confusion and help to some extent.
Like • Show 7 Likes7
Actions
Snehal Shah Nov 4, 2018 7:11 AM
Mark Correct
Correct Answer
Daniel you must be aware that draft is a taper given in vertical faces w.r.t. parting line for easy withdrawal of die/pattern from mould.
These are basic foundry shop terminologies.
There are 3 types of draft.
1. Negative draft
2. Positive draft
3. Positive-Negative draft
1. Negative draft reduces basic dimension within permissible tolerances. (refer ISO 8062).

2. Positive draft adds to basic dimension, which can be removed later on by machining or grinding process.
3. Positive-Negative draft is a combination of both types. Where height dimn. is much more after parting the job; giving it -ve draft will result in heavy reduction in material at top or giving it +ve draft will result in heavy extra material at parting line. To compensate this +ve-ve draft is given.
Reference angle is nothing but draft angle w.r.t. parting line.
Hope this helps.
If you still have any questions regarding foundry/castings/moulds....just knock-knock.

regards,
Snehal
Attachments
- DRAFT IN MOULD.SLDPRT.zip113.0 KB
Like • Show 4 Likes4
Actions
Ruben Balderrama Nov 5, 2018 8:25 AM
Mark Correct
Correct Answer
Buy a book
Gastrow Injection Molds: 130 Proven Designs: Amazon.es: Peter Unger: Libros en idiomas extranjeros
You can design a product with negative and positive draft angles.
Wich is the difference? Cost/Money/Cheaper.
You on design has some restriction like that, on construction you don't have restriction, because you need to make it able....
Like • Show 3 Likes3
Actions
Ruben Balderrama Nov 5, 2018 8:25 AM
Mark Correct
Correct Answer
Here you got something else
https://www.rtpcompany.com/wp-content/uploads/RTP-Part-Design-Guidelines-for-Injection-Molded-Thermoplastics.pdf
https://www.stratasysdirect.com/-/media/files/direct/design-guidelines/injection_molding_design_guidelines_2017.pdf
How to design parts for Injection Molding | 3D Hubs
https://medium.com/jaycon-systems/engineering-guidelines-to-designing-plastic-parts-for-injection-molding-1c554a4545be
http://files.hanser.de/Files/Article/ARTK_LPR_9783446215870_0001.pdf
Like • Show 3 Likes3
Actions
Doug Seibel Nov 5, 2018 9:13 AM
Mark Correct
Correct Answer
Reference Plane:
Movement of the mold/action will be perpendicular to this plane. It is also commonly called the "Pull Plane". The "direction" is normally set so that the arrow is pointing to the cavity-side of the mold or, in the case of side-pull action, the direction of retraction.

Positive Draft:
Often referred to as "Cavity-side" draft.

Negative Draft:
Often referred to as "Core-side" draft.

Molded parts must have draft. Faces/surfaces that are perfectly vertical from the reference plane are something that is exceeding undesirable. Everything needs draft...some things need more draft than others.

For instance, take a look at all the plastic in your vehicle...the dash, the steering wheel, the door panels, the glove box, and so many other things...do you notice how many of them have some type of "texture" to them? Some have a texture to make them look a bit like leather, some have a smooth but dull or matte satin finish...every single plastic item that you see has some type of intentional texture on it. Different textures require different minimum angles to release from the mold without the mold causing damage to the texture molded onto the plastic part.

Another critical draft is where there are "jogs", "jumps", or "transitions" in the parting line surfaces. Angles of 3 degrees or less are what is known as "self-locking" angles, and need to be avoided.

Self-Locking Angles/Tapers: Angles of less than 3 degrees per side. Some use the "rule of thumb" of 7 degrees included angle, or 3.5 degrees per side. If you grind a tapered pin with 2 degrees per side draft on the diameter, and put it into a mating hole that has the same draft, it will "lock" into the hole. It will take significantly greater force to remove the pin, than was used to install it. This condition is extremely undesirable/destructive on a mold. Conversely, there are Self-Releasing Angles/Tapers...which are simply angles greater than what would be a Self-Locking Angle/Taper. Grind a tapered pin with a 5 degree per side draft on the diameter and put it into a mating hole that has the same draft, and the pin will fall out of the hole if you turn it upside down and let it fall out...beat on it with a hammer and turn it upside down and it will still fall out freely. Self-Locking Angles are very bad in a mold, Self-Releasing Angles are very good.

The draft analysis tool in Solidworks help you identify whether or not the part is drafted properly for being molded.

FYI...
The default Green/Yellow/Red coloring setup is, imho, very limited in is usefulness. I recommend changing the Red to Blue, so that it will be more useful when you click on "Gradual transition". Only use the "three color" draft analysis for making sure textured surfaces have enough draft and parting line jogs have enough draft. The "Gradual transition" allows you to better see everything else (like back-draft, undercuts, zero draft, etc.).
Like • Show 5 Likes5
Actions
Steven McCallion Nov 5, 2018 9:35 AM
Mark Correct
Correct Answer
This is one of those things like word mispellings that I've just given up on in my life, because no matter how much effort I put into trying to remember it I just end up forgetting it anyway the next week; trying to remember if separate is seperate vs separate for example. Thus when I use the draft tool I set the draft to a big number where I can see clearly on the screen that it's drafting in the correct direction, and then adjust appropriately.
Such a rebel.
Like • Show 3 Likes3
Actions
Daniel Sevier Nov 5, 2018 1:25 PM
Mark Correct
Correct Answer
Thanks all for your helpful input.
I guess I still have some confusion, so I have some put some images here to consider:

So, this is the "reference angle" to which I was referring:

I'd like to understand this reference angle relative to the reference split plane and relative to the part's facial draft angles.

You can see in my example model (with 15 degree drafts on faces) that as soon as 15 degrees is exceeded in the reference angle, then the face turns yellow (from green with a positive draft), indicating that it needs more draft. I'm finding it difficult to visualize why this would be a problem. (You can see I just input 15.01 degrees as the reference angle to test this.)

So, if the orange angle is the reference angle and is greater than the facial draft angle, how would the parts get stuck? (or do I have it drawn wrong?) Thanks for your help!!
Like • Show 1 Like1
Actions
- Deepak Gupta @ Daniel Sevier on Nov 5, 2018 1:57 PM
  Mark Correct
  Correct Answer
  Please do not get mixed up with the draft analysis and mold. Draft analysis is a way to find any faces with less draft (means small angle value vs the specified value; so 15 vs 15.01 in your case), faces with no drafts or faces with draft in reversed direction (positive or negative draft) instead of in correct direction (in simple words, face have negative draft when positive was required on that face or face have positive draft when negative was required on that face).
  
  Now since required draft is 15.01 (as you've specified), the draft analysis tool is indicating the faces (using yellow color and marking them under required draft) that have less draft angle than the specified value
  
  Based on the following picture, you've drawn the reference angle correctly. The part won't get stuck in the mold since it already has some draft but molded part dimensions may not be correct since the reference angle (required draft value, 15.01 in this case) is not same as on the part (given drat value, 15 in this case).
  Like • Show 4 Likes4
  Actions
  - Daniel Sevier @ Deepak Gupta on Nov 6, 2018 10:45 AM
    Mark Correct
    Correct Answer
    Thanks Deepak! Makes much more sense now!
    Like • Show 1 Like1
    Actions
- Doug Seibel @ Daniel Sevier on Nov 6, 2018 8:48 AM
  Unmark Correct
  Correct Answer
  Daniel Sevier wrote:
  
  Thanks all for your helpful input.
  I guess I still have some confusion, so I have some put some images here to consider:
  
  So, this is the "reference angle" to which I was referring:
  
  I'd like to understand this reference angle relative to the reference split plane and relative to the part's facial draft angles.
  
  You can see in my example model (with 15 degree drafts on faces) that as soon as 15 degrees is exceeded in the reference angle, then the face turns yellow (from green with a positive draft), indicating that it needs more draft. I'm finding it difficult to visualize why this would be a problem. (You can see I just input 15.01 degrees as the reference angle to test this.)
  
  So, if the orange angle is the reference angle and is greater than the facial draft angle, how would the parts get stuck? (or do I have it drawn wrong?) Thanks for your help!!
  
  The "Reference angle" is nothing more than a value that YOU set.
  
  Let's say, for instance, that I am tasked with designing a mold for this part...
  
  And when I go over the finish requirement for this part, I learn that they are wanting to have a specific "leather" texture on all the "show" (visible by the end user / customer) surfaces. I quickly check and find that the minimum draft required for that specific texture is 6 degrees. So I launch the Draft Analysis tool, select the proper reference plane, and enter 6 degrees for the reference angle. Now, any area of the part that has less than 6 degrees draft, Solidworks will color yellow.
  As we can clearly see...the part, as currently designed, has areas that do not have enough draft for the desired texture.
  (One thing that is important to note regarding the "Reference Angle" in relation to the "Reference Plane"...Zero degrees is perpendicular to the Reference Plane, NOT parallel.)
  
  So now I can quickly go back to the customer and show them that their part does not have enough draft for the texture they had originally desired. At this point, they could choose to change the part model to allow for the desired texture, or they could change the texture specification to accommodate the existing part design.
  
  The "Reference Angle" can be any value you desire/require.
  Like • Show 6 Likes6
  Actions
  - Daniel Sevier @ Doug Seibel on Nov 6, 2018 10:45 AM
    Mark Correct
    Correct Answer
    Thanks! Makes much more sense now with the clarification about the reference angle being what I choose to set.
    Like • Show 2 Likes2
    Actions

Meaning of Negative & Positive Draft Angles in Molds?

Attachments

Outcomes

Attachments

Related Content

Recommended Content