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Combining or merging two random surfaces on model.

mmelenli
4-Participant

Combining or merging two random surfaces on model.

Hello everyone,

 

I had some advices about this specific part im sharing before, but I couldn't manage to do what I exactly wanted.

You can see in the pictures there is a gap between two areas I marked, You can also find that part in the attachment.

 

How can I close that gap with everywhere having 2mm thickness (that gap too, if those areas can be merged.)

 

You can see what I'm trying to do here, from the previous thread of mine. 

https://community.ptc.com/t5/Part-Modeling/Managing-thickness-of-an-igs-file/m-p/612959

 

Best Regards.

1 REPLY 1
tbraxton
21-Topaz II
(To:mmelenli)

I am not able to open the part file in Creo 4 but did look at the IGES geometry. This appears to be a volute design. Volute modeling is often non trivial when it comes to creating the geometry of the tongue and the blend from the outlet to the spiral. This may well be a case of fixing the bad import geometry would take longer than building the geometry in a way that supports what you want (thickness of 2mm throughout). I see issues with the import data that will make what you want to do difficult and tedious. It is not an accuracy issue it appears to be a geometry issue in that the import geometry does not enable offset to a thickness of 2 mm. If I had to do this I would build the geometry from scratch so that it would thicken as required. Assuming that you know the design parameters for the volute geometry I would suggest you build it from scratch.

 

If you have control the source geometry used to create the IGES data then I would build a model knowing that you need to thicken it. Build all of the following as surfaces that will create a closed quilt defining the control volume for the volute. Offset the features as you create them to insure that they enable your offset thickness requirement, don't wait until the model is done to offset it and find out it does not work. See the pics in the zip file for more detail.

 

1) The spiral of the volute can be built by defining a sweep trajectory using curve from equation. This looks like a logarithmic spiral for which the equation is straightforward using cylindrical coordinates.

 

2) You can then use a variable section sweep along this trajectory to create the spiral volume.

 

3) Create outlet geometry that comes short of  intersecting the spiral

 

4) You will then need to create blend geometry between the outlet and spiral quilts, this is the most difficult part. I would use Creo ISDX  to make these transition surfaces which makes it easier and faster.

 

5) Offset quilt to thickness

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Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
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