Mold maker blowing smoke at me?

I'm having to deal with a difficult person -- a mold maker favorite of my client who likes to make me jump hoops to please him. (Actually he's
not such a favorite any more, because our common client now understands how difficult he's being.) He's telling me something that might be accurate, and might just be his way to make life difficult for me. Basically his story is that when metal is passing metal in a core/cavity that they need 10 degrees draft between the two surfaces, otherwise there is a high degree of danger that the mold will lock up at some point. I've got no special difficulty believing him, on the one hand, but I'm suspicious. I wouldn't have thought quite that much draft would be necessary. I'm going to have to do some thinking about how to accomplish it in the particular application I have. You can see the area of the part by going to:
http://www.h2omarkdesign.com/img/connector_ring.jpg
I have annotated the area in question. Any comments? Experiences to the contrary? Doubtless I'll give him his requested draft anyway since we don't want to give him an excuse to do a poor job, but we're probably going to be moving to a different mold maker soon just because this guy is so difficult (not specifically because of this issue, but on a number of different issues).
TIA Mark 'Sporky' Stapleton Watermark Design, LLC www.h2omarkdesign.com
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ho Sporky, I usually get away with 5 degs for designs like that. Obviously the 5 degrees only needs to be wehre metal meets metal, so it doesnt affect the standard draft for the plastic sides. what natural angle does it work out to with the gap you have given hime between the 2 vertical faces? I have occasionally negotiated even smaller drafts with the toolmakers for those situations, but if there's no reason not to, I generally try to give them as much as possible as long as it doenst affect the design. Sounds like he may just be difficult, if he's not willing to compromise. Olaf

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Aside from the fact that I got this when I tried to look:
403 forbidden
Server configuration does not allow access to this page. Please go back and try again.
Send it by email.
The tangent of 10 degrees is .17, very close to the general coefficient of friction for steel on steel. So you can't argue that 10 degrees wouldn't be generally safe against lockup. But there are many other factors to consider too.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Funny -- it does that to me also sometimes. But then if I just paste the link into my browser it comes up fine. I don't really get it. Guess I'll ask the folks at my Web hosting service.
"P." wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
"P." wrote:

I've never heard of this. What does the tangent of an angle have to do with the coefficient of friction of a material? Static or sliding?
Hoping to learn something new.
-Martin
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Dig up your old physics book.
The friction coefficient is the ratio between the friction force and the normal force that generates it. The two forces are perpendicular so that ratio is a tangent (rise over run) if you draw the force vectors out. So if you put a box on an incline and raise the incline angle to greater than the arctan of the friction coefficient the box will begin to slide.
In this case we want the box (mold halves) to slide past each other so the draft angle should be greater than the arctangent of the friction coefficient. Steel on steel typically is taken as .2 which is a little more than 10 degrees. Polished hard steel on hard steel, perhaps with a little chrome plate or electroless nickel will probably be less.
Martin wrote:

coefficient
do with

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Tapers that are more shallow than a certain angle (for example the Morse taper in the quill of a drill press) are self-holding. They're around 2.8-3 degrees.
Best regards, Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
snipped-for-privacy@interlog.com Info for manufacturers: http://www.trexon.com
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Our mold is harndend steel. I will check it out monday, and see if we used 10 degrees I could have recalled wrong. Other then that I have read many books and also just learned from experience on the cooling, venting, and material flow.
The manufacture of the plastics sometimes have some very detailed callouts on the required flow paths, cooling, and venting and they specify it for the exact material being used. Another good book 'On the Road with Bob Hatchet," he has some good insight to the issues he ahs found and solved in the field.
When I design the part I have molding in mind and also mold making because I also create the NC code for cutting the mold in the CNC. When I am designing the mold I always have the cycle of the part in mind. Say for instance, I have had molds that I have had to slow the cycle on because the part was getting pin push from not have enough or large enough ejector pins. So I design with plenty of pins. Another popular issues is the mold designer's desinging small sprues and runners thinking that it saves material. Saving the slight bit of material does not come close to saving money if the cycle time is increased to make good parts, or the bad part scrap rate is higher. If the sprue is small, and the gates are small then the pressures are very high on fill and usually you have a smaller window for molding. If I save material on the sprue but my scrap percentage on the part is 10% then I have not saved anything. Anyway I could go on forever, I am passionate about this issue.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Hi,
We have designed many, many such parts, and use 5 degrees as a 'rule of thumb'. Depending on how many parts you need to get out of the tool, and the contact area between the tool faces in this area, you can even use as little as 3 degrees - but it's risky.
I've found that most suppliers will recommend the absolute max. for just about anything: sheetmetal bend radii, part wall section, tool steel shut-off, draft angle etc. Experience shows that nearly all of these rules can be broken.
Regards,
Anthony
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Spork,
I use 5 degrees as well.
After looking at your picture, it should be plenty.
Regards
Mark

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Mark, I too, have used 3-5 degrees, but I try to keep 5 degrees so that I don't have as much chance for the ever-so-slight misalignment on close that can cause frettting wear.
On mating surfaces of conical stripper rings I keep 10-15 degrees.
Fretting with materials of the same hardness is common, so the toolmakers I have worked with always have recommended nitride on one surface and a different hardness on the other surface makes for longer life.
I must admit I have left these decisions to the toolmaker's discretion except when the angle was critical to achieving design intent. I have an exact equivalent of that in one design right now where the flow area I need given the limiting ANSI standard fittings required will demand I use 3 degrees on core shutoff. I will ask for a carbide face on one surface or the whole core pin.
Bo
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
That's some interesting info about the different surface treatments -- makes perfect sense to consider that to help prevent galling. I'm not going to tell this guy his business (although he tries to tell me mine), but I'll remember the concept. Thanks (to all who reply also).
Bo wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Sporkman wrote:

<snip> We use different hardnesses to prevent galling as well. Makes a big difference.
Mark B.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
I design molds and I would say you could use 5 degrees in that situation. We have similar parts that are single thread nuts and we have had to do the same thing. We have so far ran about 10 million parts with no trouble. But again with not doing the whole design I could be missing something. I would say it is good he is at least giving you a heads up. Maybe ask to go see his design and talk it over.
The biggest problem I had before I designed our molds is that my molds were being made by very good machinist who did not understand molding our how the material flowed in the mold. Did not understand venting and cooling. I was a Plastics Process Engineer before I designed molds. In fact I still am the one to dial the molds in after we make them.
Sporkman wrote:

of
he's
understands
core/cavity
hand,
would
since
probably
guy
number
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
grantmi1, I was glad to see your comment on knowing about material flow, venting and cooling.
I have had a situation where a toolmaker-designer (so-called) claimed he was doing a proper cooling design on a 4 cavity mold and in fact after the mold ran, it was probably 35% longer cycle time than everyone thought it would be (& experience showed possible).
Is there a book on mold cooling design where I can gain more insight into the subtleties? I know that there are mold cooling analysis software, too, but that only analyzes what you throw up on screen, so that comes later, if needed.
Thanks - Bo
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
The SPI website has tons of books and might be worth joining if you want to network with plastic mold types.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Bo wrote:

Some good rule of thumbs stuff can be found in Bill Tobin's books: http://www.wjtassociates.com/page/page/1168073.htm
I also have links to good free resources on our site: http://injection-moldings.com/faqlinks.html look at the references section. Most of these links are plastics design but some have tooling issues.
Mark B.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Never had a moldmaker squawk about anything down to 7 degrees for passing cores. 3-5 degrees was almost always doable in situations that required it.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Never had a moldmaker squawk about anything down to 7 degrees for passing cores. 3-5 degrees was almost always doable in situations that required it.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Anything under 10 degrees is approaching lockup. Other factors need to be considered such as surface roughness, material types in contact, finish/coating. In general, I would have to agree with your mold maker and avoid the potential for problems. Sometimes you might be OK and others not. As P already pointed out, the tangent of the angle should be greater than the coefficient of friction between the two materials in contact. This is analogous to a worm-gear pair, if the tangent of the thread angle is less than the contact coefficient of friction then the worm gear cannot back drive the worm.
Kman

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.