Unable to split a body using plane

[HK_13985408]

Creo Parametric version 8.0.7.0

I'm trying to create a mold for my subject and want to split the body using a plane. Which fails.

Then I tried to extrude a body out of the plane I want to split, and the use boolean operation feature to either intersect or subtract the bodies. I was successful on one side, but the other side fails, which I believe the same problem it may have faced when splitting using the plane.

Any advise, help is greatly appreciated. Thank you! Fails trying to split using a planeOne side successful using another body to get the intersectOther side fails trying to do the same operation.

[tbraxton]

If you are using a commercial license (not educational) then post this model here for review. Determining the issue is not easy without access to the model.

[HK_13985408]

Hi! Apologies for not replying sooner.

I tried to upload the part to this thread. But I get this error message instead. 

" The attachment's ptccommunity.prt content type (application/octet-stream) does not match its file extension and has been removed." 

[StephenW]

Zip the file and attach.

[HK_13985408]

This is the part attached. There are some external dependencies as I drew it using an assembly. I removed them so it can be independently generated. 

[tbraxton · Accepted solution]

Change the accuracy of the part from 0.01 mm to 0.001 mm, regenerate the model and then create the split feature, it should work.

[tbraxton]

The issue was created by round 2, it creates a geometry artifact that results in a small edge when the split body feature is applied. That spherical well should be created to avoid this unless your design intent was to create that small flat between the holes.

Did you come to Creo after using Solidworks prior to working in Creo? I am asking because you have externalized sketches on most features, and I am curious as to where you were taught to do this. I am not insisting it is wrong, but it is something I have to deal with from time to time with users and teaching the efficient and optimized implementation of design intent within Creo when modeling standards are enforced in some organizations.

[KenFarley]

We had some guys who went to Creo training and they were apparently taught this "make a sketch, then make the feature that uses the sketch" technique. I don't understand why this philosophy was adopted, except to perhaps soothe people from other software packages that use it. It makes model trees at least twice as long as necessary with no really discernible benefits I can see. I'll use a separate sketch if the geometry defined is going to be used in multiple features, but otherwise I don't do that. Is it a matter of personal preference? Perhaps. But I definitely find it more understandable and "neat".

[StephenV]

I have to support your input on embedding sketches in a command versus sketches outside your command. All you state is so well said, and many Creo instructors enforce the best practice to embed your sketches. Yes, sketches outside make model tree extra-long and less neat. Also, you have better down the road integrity if the sketch is embedded within a command. Low risk otherwise outside, but if you have very large number of commands in your tree and you manipulate that tree you stand a higher risk of issues that could develop, and that you have to chase those issues. Plus, at low risk, that sketches outside command 'might' have less direct tie to the command in the world of unseen algorithms. I've taught CAD and PTC products for decades in college and workplace and like many other instructors I prefer to embed your sketches as a best practice. Again, though it does depend on your application and use of sketches for multiple commands.

[HK_13985408]

How else should I make different features on different planes? I always thought of it as a make-it-happen-as-you-go-along approach

[KenFarley]

How to make a particular feature depends on what that feature is. If a feature needs to have different depths from a surface, and you are defining each depth's shape using extrude features, you need the shapes at each depth to be defined in their each separate features. The decision of which feature to do first, which is next, etc. depends on what I'm trying to achieve, which features need to intersect others, and any other concerns. My general approach is trying to have a minimum of features, a robust as possible. I'm always thinking how easy or difficult is it going to be on me if I need to change any of the features I'm building, too. This happens a lot when developing things,

There are a lot of considerations I take into account when defining geometry that are learned from pain in the past.

[HK_13985408]

Thank you for the explanation. I managed to split it after changing the accuracy.

And yes, I am very new to Creo and I got the roots from SolidWorks. What do you suggest as the "better" approach when working with Creo? I always thought it's just easier to sketch on the plane I need the change.

[tbraxton]

IMO it is not a best practice to externalize all sketches, but I see it with increasing frequency. In most cases it is because someone was using SW before coming to Creo, but it appears some Creo training classes are now teaching it as well.

If you adopt the strategy of minimizing/simplifying parent child relationships when modeling, then one would use internal sketches within feature creation whenever possible. As complexity of designs grow (increased feature count) you will benefit more from following this strategy. You could probably rebuild the model you posted here and cut the feature count by 50% and still maintain the same design intent.

As a general rule I would only use external sketches if that sketch would be a parent to two or more children. Creo has internal sketches embedded in many feature creation workflows. You will be presented with the option to define the sketch within an extrusion for example so there is no need to create the sketch before creating solid geometry in many cases. 

Be aware that when in sketcher mode there are many ways to create references to features/geometry that were created prior. If you explore this concept, you will see that you will not commonly need the external sketches that you are currently using to build additional geometry. The most important consideration when sketching/making new features is to build them such that the design intent of the model is accurate and minimizes external references.

[Michael]

Check your accuracy.

If you don’t want the other side you can select the plane and choose solidify.