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J
JC_105098271-Visitor
1-Visitor
November 29, 2022
Question

Help with Swept Blend

  • November 29, 2022
  • 5 replies
  • 5490 views

Hey all, first post here. I am trying to use the swept blend feature to remove material as shown below. I am using a start sketch and an end sketch to drive the geometry of the swept blend and I am using a curve that I created by points (many!) on the outside surface of the original geometry. The issue that I am having is the swept blend is not working very well and leaving a lot of excess material. Also, it is not following my curve very well. I tried using two trajectories but I do not think that is allowed. I have been struggling with this for may days now so any help is appreciated. The end goal is to remove material from the center section and have it tapered on the edges at like a 45* angle, which you can see from sketch.

5 replies

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
November 29, 2022

The most likely issue is that your blend vertices are not mapped correctly, or your sections do not all have the same number of sketch segments.

 

When using a swept blend each section needs to have the same number of segments and the blend vertices often require manual intervention to map them to get the desired geometry.

 

Step 1: Confirm that all sections have the same number of segments

Step 2: Query the blend vertices and remap as required once step 1 is validated

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
November 29, 2022

Watch this video for explanation of the requirements for swept blends.

 

https://www.youtube.com/watch?v=4t14TgzONh8 

K
KenFarley21-Topaz II
21-Topaz II
November 29, 2022

A few possible observations:

(1) Is your accuracy set to some sort of absolute value? Often these kinds of things are made impossible because of accuracy settings that aren't good enough.

(2) If you can extend the definition of your swept blend so it extends beyond the outer surface you're trying to cut, you will make your life a lot easier. Attempting to build a surfaced model that exactly corresponds to another surface is wishing for a lot. Local changes in curvature can cause the surfaces to not intersect at different patches, leaving the kind of thing seen in your image.

J
JC_105098271-VisitorAuthor
1-Visitor
November 29, 2022

That is what I was thinking. I bet I can offset the surface then base my curve off that surface so that my trajectory is beyond the surface I am trying to cut. I will report back if it works.

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
November 29, 2022

If I understand your design intent, there are easier and more robust ways to remove the material shown in your picture. Can you post the model? Make sure to note what version of Creo you are using.

J
JC_105098271-VisitorAuthor
1-Visitor
November 29, 2022

I am using Creo 6.0. I can confirm that all the sections have the same number of segments. I would like to complete this task myself but if I cannot get it I am open to having you help. Is there any way you can communicate the process you would follow to complete this?

Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
November 30, 2022

In looking at it I'm not surprised.  Creo interpolates everything between fixed sections, so, it's only accurate at the sections themselves.

 

Use a variable section sweep with multiple trajectories, and make sure the trapezoidal section actually sticks out of what you're trying to cut.  When the longest edge of the trapezoid is exactly coincident with the surface you're trying to cut, sometimes, the absolute accuracy becomes an issue as mentioned by Ken.  So, if that longest edge is ALWAYS outside of the part, it will cut better.

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