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Variable Round

DieselPig
1-Newbie

Variable Round

Morning All

Been trying to get a 12 mm round on the attached drawing. Tried the surface to surface and even this won't work. any experts care to point me in the right direction?

Many Thanks.

1 ACCEPTED SOLUTION

Accepted Solutions

I was able to create a constant 12mm round now.

One more thing. I have excluded 2 pieces from the chain so the blend is smooth:

View solution in original post

17 REPLIES 17

See attached.

Hi MRV

When I try that on my PC (Creo 3.0 M090) it fails at 12 mm, 10 mm is OK.

I have reordered the rounds.

First the 12mm round and then the 5 mm rounds.

I have used 12mm all over and 5mm only at one end.

Hi MRV

I can see it now but, how did you select the chain in the references? When I try this I only get an edge.

Select one edge then hold shift and select the remaining tangent edge.

or for non tangent edges, hold CTRL and select all the edges.

I can create a chain but have you done this in a particular order? I have tried to copy your selection but my results are different!

I usually select edges in an order.

For a chain you need to select the tangent edges in an order.

Also in this case since you have used surfaces, the edges are not tangent all over. you need to select the missing edges along with the chains.

I was able to create a constant 12mm round now.

One more thing. I have excluded 2 pieces from the chain so the blend is smooth:

Hi MRV

I have tried to copy what you have done without success! No matter what I try I cannot get the same result. Are you using a later release of Creo 3.0 ? we have M090 here.

Iam using Creo 3.0 M110.

Hi MRV

I have finally solved it!

Looking at your picture and removing the two sections and it has worked.

Many Thanks for your help.

creodential
5-Regular Member
(To:DieselPig)

You have to switch the order of the 5er and ther 12er, yes, but that didn't cut it.

I had to add the highlighted rounds in order the get a working continous surface-surface round 12 (three sets needed).

No errors in the geometry check.

ScreenShot00440.png

Your problem arose from non tangency conditions in your sketches.  Primarily SKETCH 1.  Then by projecting you just transfer this non tangency along through all the features.  You should have used splines to create the veins or converted all the segments to a single curve this would have helped.  I reworked your file.  It is attached.imp2.jpg

Hi Ron

Thanks for that, how did you convert the segments to a single curve?

There are two ways

1st this is what I did.  I went in and redefined your sketch, I selected everything you had sketched, except for the small round on the inside tip of the vein.  I then right mouse button and turned all your arcs into construction features.  Then from the node of the small round left over I started drawing a spline. It was snapping to your construction curves, I put maybe 3-5 points along the length of the spline.  When finished I chose the constraint for tangent and then forced the spline to be tangent tot he curve at the tip of the vein.  Then I went and removed all the constraints on the points of the spline releasing them from your construction geometry. I did the same thing to the other side of the vein and finally I put an arc for the outer most diameter from the center to the end points of the 2 splines.  I did this for both your projected Sketch 1 and then for the lower flat sketch.

Alternately you could just covert your geometry directly into splines by edit definition of your curve then select with cntrl all the lines you want to make into one spline.  Then click the operations menu and convert to tab then spine on the drop down.  I did not use this on your because you had some of your curves that were not tangent which would still make for a poor surface quality when making your round.  spline.jpg

Hi Ron

Just tried this method on a new impeller I'm working on with the same issue and it worked!

Wow, again I learn a new method.

Thanks for your input, very much appreciated!

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