How to make offset inside sketch parametric stable?

[pimm]

I would like to be able to offset a curve enclosure inside of a sketch and observe the change's relation to the geometry outside of the sketch.

Is there any way inside of a sketch to use the offset option and have the offset recognized as a offset instead of the resulting geometric features created from the offset?

Below is my simple sketch prior to the offset.

Below is the application of the offset.  Notice that the offset is recognized as 2 weak radii shown in light blue.  This applies as it should.

The problem is that if I modify any of the strong dimensions the needed offset is no longer uniform.  (Below I modified the angle value).

Perhaps in this specific example it would be possible to modify the constraints to get the needed offset with the change, but in a more complicated sketch I would like the option to have my offset features retained as a offset as I have intentions of having this update appropriately with the downstream extrude within a family table.

[tbraxton]

Getting the sketch constraints to support this is the trick. This is not the only way to get a solution, one example.

This example Creo 7 model enclosed will support your goal but does not use the offset function exclusively. There is a part parameter SK_OFST1 that is used to define the offset value and this parameter is used in feature relations driving the sketch along with constraints that ensure the offset behavior is enforced. These are datum points at the midpoint of each arc being offset with a linear distance between them. These linear strong dims control the offset within the sketch via the feature relations. The user can change the offset parameter value and regenerate the model without entering sketch mode.

[pimm]

Tbraxton:

Even though this doesn't solve a true offset it is quite helpful.

The only way that I have been using relations is where one feature in a sketch gets assigned a name and is referenced in another sketch.

This idea uses the relation table.

I could see that both .850 dimensions in your sketch were relation driven.

I am new to this style of relation so I have a couple questions.

1) To build the cooperative number between d9 and d10 do you just build this relationship by typing in these names and the = sign?

2) Is the SK_OFST1 value actually functional or is it just a name that could be used downstream in a family table to give name definition to the needed offset value?

Thank you,

Paul

[tbraxton]

1) The feature relations for d9 & d10 were manually typed in the relations editor including the = sign.

2) SK_OFST1 is a model parameter and is functional it is used in the relations to set the offset value. You can see this parameter using the parameter editor by using: Tools-> Parameters.

[KenFarley]

A method I've used is to employ construction circles, tangent to the "offset" pair of entities, to make the profile more reliable. For example, for your geometry, I constructed the sketch shown below. Outer profile constructed as you defined, inner circular entities a concentric with their corresponding outer edges, tangent to the construction circles. Construction circles are the same diameter. Seems to work very well, and there is only one "offset" dimension defined between two of the arcs.

I use this construction circle "trick" quite a bit to space things out, it's often helpful in keeping things spaced evenly, especially in situations where there are not explicit curves that can be set to the same length, etc.

[kdirth]

Another option to keep all of the offset values the same is to use the equal constraint on the offset dimensions.  This will leave you with one dimension and multiple "equal" dimensions (E1).

[pausob]

I tend to use perpendicular construction line segments + the equal length constraint in order to implement the design intent in these cases:

 

[pimm]

It appears that there are a number of good ways to maintain equal size offset in my given circumstance.

It would be nice if there also was a way within a sketch to just automatically carry the offset values driven by the offset value that was assigned to a given profile.

[tbraxton]

Here is an alternate solution using two sketch features and the offset loop functionality. This does not require any relations or parameters and allows for modifying the offset value without entering sketch mode. This is the simplest implementation I can think of to capture the design intent. Sketch 2 is offset from sketch 1. The offset is controlled by a single dimension in sketch 2.

Creo 7 model enclosed for reference

[pimm]

Perhaps in the above instance you could use a shell command with your extrude to maintain the needed offset.

[tbraxton]

Sorry, I do not follow your comment in the context of the alternate solution. There is no 3D geometry in the example part, only 2-D planar curves. If you are asking about a scenario where you are using this offset to control thickness in a 3D model then my answer may be quite different on how to capture the design intent.

[pimm]

The next step beyond the sketch would be extruding the offset sketch as a solid.

Since your above sketch didn't have an internal offset I thought the next step would need to be to build the offset as a solid.  (I should have said thicken instead of shell). 

[tbraxton]

In that scenario, this is how I would construct the 3D solid using a single feature. No reason to have any external sketches to create this geometry.

Use this sketch:

To extrude a thin protrusion explicitly controlling the thickness

[pimm]

Very good.

Now I understand. 

The sketch that you built off of another sketch looked like it just had the original profile as construction lines. 

This would be a fairly good option as well if the original sketch was more complicated.

[pimm]

As a summary to my original question:  How to make offset inside sketch parametric stable?

Even though it is possible to work around this, it isn't possible to parametrically hold the geometry as an offset value within a sketch.  (Each segment of the offset has it's own independently determined parametric value).  This means that if you want to observe the downstream effect of the offset within a sketch within the model tree that you can't change the offset value inside of the sketch without 1st destroying the outer offset the next time you enter the sketch.

It would be wished that it would be possible to at least have an option to keep the offset geometry within the sketch as a complete offset value that could be changed with just changing the original offset value.

[Dale_Rosema]

If want your wishes to come true, you could start by adding a product suggestion:

https://community.ptc.com/t5/Creo-Parametric-Ideas/idb-p/creoparametric

[pausob]

Hi @pimm , I'm not quite sure what you mean about impossibility of parametrically holding the geometry as an offset value from other geometry / destroying the outer offset the next time you enter the sketch.

Several examples were shown where that is very possible.

So I suggest you file a product idea about it, and document it clearly and explain why this would be desirable.

Still, I wonder whether implementing such idea is not worthwhile because already existing tools and workflows achieve the design intent fairly efficiently.

[pimm]

I'm not knocking any of the ideas submitted.  I gave many of these ideas Kudos because they would certainly work given the context of the given simple sketch.

The idea given by Tbraxton towards using one sketch to drive an offset in another sketch is as close to solving what I would like to see.  We do use this method very frequently.

I just wish that since within a sketch since there is an option to offset the curves in that sketch that the geometry within that sketch could at least have an option to assume this specific type of parametric which would keep it more stable than the default parametric's.

We don't often have cases where we build parallel extrudes plus the fact that zero of my idea submissions have been adopted by PTC so I stopped submitting them years ago.  PTC doesn't listen to the little guy.

[StephenW]

Quick correction here...sorry...the fact checking alarms went off and it needed verified....

Fact check:  @pimm stated "PTC doesn't listen to the little guy."

Result: FALSE

Verified statement by multiple sources:  PTC doesn't listen to anyone.

Ok, crisis averted, continue with your day.

😀😁😂🤣

[pausob]

Well, yes, no arguments there from me about PTC "not listening".  Though I will say there are people within PTC that are trying to change that reputation.  

In my opinion, the offset functionality "works to specification", but what I think is missing is the the lack of an "composite curve" or "polyline" type of an entity when sketching.

I think such a "smart-chain", identified by its starting and ending segments would conceivably be offset with a single number, and the number of segments in the resulting curve would be varied as needed - for example, the corner radius arc would be automatically deleted if the offset was too far "inwards".  This is actually what happens now with the @tbraxton 2-sketch method - basically, because the system treats the 1st sketch as a composite curve...

Anyway, having this at the sketch level would streamline the design work, make the perimeter dimensions easier to apply, and maybe make it easy to re-route mutli-segment loop sketches (I do dread having to one-by-one re-route individual segments and hope I picked everything in correct order)

[pimm]

I guess that when I asked the question about whether Creo could apply internal offset parametrics within a sketch I kind of expected that this wasn't possible but I just wanted to make sure I wasn't missing anything.

Normally I wouldn't have a offset set of curves that I would want to directly extrude but if parametrics within a sketch were more stable on more complicated sketches there would certainly be applications for this.

We do use the TBraxton offset by 2 sketch method frequently but sometimes the offset sketch doesn't hold together well if a change was made to the 1st sketch (even when replace is used)..

I too struggle with complicated multi segment loops in getting everything to work correctly.

Thank you all for your help!