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Draft Analysis


Draft Analysis

Okay.....I have to ask this again. Have we totally lost the ability to specify a two color draft analysis?

If we have, note to PTC Developers: A five color draft angle range is CRAPPY! There is no way actual plastic partor casting designers were consulted on that.

If we do still have this essential ability, please enlighten me on how to do it. I cannot change 5 to 2 in the range box nor can I effect change anywhere else that I can determine.

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Dean, To start, I have to say that I do not have an answer to your
direct question. As far as I can tell there is no way to change the color
range below 5
However, (to offer an opinion as a plastics designer myself) I'm not sure
why I would want it less than 5 colors. Personally, I set my configs
"color_scheme.txt" to show the old WF rainbow color range set at 7.
So, If I want to do a draft check to evaluate varying draft angles around
my part, I set my "Draft" range to 5 or 10, and it will show me a rainbow
of colors. If I want to do a draft check to evaluate the parting line, I
set my "Draft" range to 0.50, and it will only show me three colors. (Pink
for anything larger than 0.5 deg one way, Blue for anything larger than
0.5 deg the other way, and Green on a surface that I may have forgotten to
Simply modifying the "Draft" range number in the evaluation box works for
me because it quickly and clearly highlights problem area's, and I don't
have to be constantly messing with my "color_scheme" settings.

Maybe this technique will help you get where you want to go...
Good Luck

Bernie Gruman
Owner / Designer / Builder


Pleaseknow I am frustrated....but I consider having to compromise usingthe range to "almost" get to the split line directlysucks. I know you do tons of plastic parts (A surfaces and otherwise) so you know the pain of trying to follow a contoured split line on sweetened/visible A surfaces where the P/L flows around. With the two color analysis it was simple to trace along the blue/pink line. Now that is nearly impossible. Besides now with Creo the shading in analysis sucks out of the box. I assume I can have it shade with edges like it used to? I have not looked into it.

I hope I am just missing some customization that will get me back to a better state.


Hi Dean - Not sure what application you are trying to arrive at here: if I
understand correctly, why not use a silhouette curve to determine P/L?

Best regards

Kelly Gensley

Genz Design

Box 232

Victor, Iowa 52347

I find that, in WF5.0, that you can:
1. perform draft check shaded
2 after the model is in bi-modal colors of the draft analysis, toggle out
of shaded mode to "hidden lines removed mode"
3. you should now see the bi-model colors of the Core/Cavity Surfs plus the
edges if wire-frame with hidden lines removed.

If that helps at all.


I am not running the mold module....if that is what you are referring to. (?) As far as I know, that type of Silhouette egdeis only accessible in Moldwith the surface trimby picking a surface and a direction. Mold Design I have that correct?


Pete....the PAIN is only in Creo.

No.that is incorrect.>applications>Mold/Castings>silhouette curve>

Best regards

Kelly Gensley

Genz Design LLC

Box 232

Victor, Iowa 52347


I've done a lot of draft analyses over the years. I've always set the max draft angle to what I want to check against and never messed with the colors. If my part requires 5 degrees, I set it at 5 degrees and if properly drafted the entire part should be one color or the other. If some areas require 1 degree and others 3, I do two checks. The entire part should be two colored at 1 degree and the 3 degree areas should be at 3. That works for me.

You can create a silhouette trim without the mold package. Create a surface copy of the surfaces you want to make a silhouette curve, select the surface copy, select the trim tool and select a normal plane as your trim direction. The silhouette button on the trim dashboard ought to then be active, select it. That will trim away or split the surface based upon the projection plane. To get a curve from that you'll then need to copy the surface edges.

Doug Schaefer | Experienced Mechanical Design Engineer


I do it that way as well. But this real qualifier and genesis of my rant was two-fold.

1. The two color analysis was magical. If I was the only one that used it in the way I did...then Mea Culpa for never sharing it with my classmates. Losing that has been like getting a few fingers cut off.

2. the shading within the draft analysis does not have any edges displayed. I hope that one is simply a config. I have not found it yet. If anyone know...please throw me a life line.

So, it's not simply the "split line" I was asking about. This thread took a turn in that direction and I wanted to get it back on course.

Thanks for all the responses so far.


To your latest question, I've found that if you do a draft check while in
Shade mode, then the details of your part disappear, if you do a draft
check while in Wireframe mode, then you will see the wires under your
Pink/Blue colors.

That's what works for me... (GC-i7K machine with Quadro 4000 Graphics)

Owner / Designer / Builder

I did know that Bernie......thanks. BUT with this particular model (approaching 2500 features) wireframe gets super slow while spinning. I know it's a work around. Thanks.

No worries. Believe me, (like all the rest of us on this forum) I'm all
to familiar with the frustration that comes along with converting into

I don't know about your install, but with my install of CEP5.0 and CREO 1 Pro-Foundation/Advantage, I need TDO option to get Silhouette curves. (and a bunch of other things)

Christopher F. Gosnell

FPD Company
124 Hidden Valley Road
McMurray, PA 15317


I have received a couple of questions asking how to save and implement the
WF style Color Scheme file... So, I thought I would just share to the
group. Here Goes...

While in Draft Check, At the bottom of the "Color Scale" window...

Hit the Arrow "down" that expands the color scale settings
Click the left "rainbow" icon (this is the old WF colors)
Change the settings number to 7
at the bottom of the window, hit the "Save" icon, and save the
"Color_scheme.txt" file to your user directory.

Then, add this line to your
geometry_analysis_color_scheme j:\PTC_User\bernie\Creo2\color_scheme.txt

(Be sure to type in your proper path with file name, instead of my

Good Luck
Owner / Designer / Builder

On Thu, Nov 7, 2013 at 12:09 PM, Bernie Gruman

> No worries. Believe me, (like all the rest of us on this forum) I'm all
> to familiar with the frustration that comes along with converting into
> Creo2.
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