I made a list of the questions that most puzzled me ! Anyone help ?

[Walker]

I made a list of the questions that most puzzled me, I would be grateful if anyone could help me with any of the following questions, Thanks

############################################

■Q1: How to scale each body or surface individually? The "operations/scale model" command will scale the entire part (all body). The "Flexible modeling/Move feature" command only can move and rotate.

############################################

■Q2:How to get these three red isolines from green surfaces?

The command under the"Style/curve from surface" only can extract isoline from a single surface, just a partial segment. Even if I extract isolines face by face, the joints of partial segments must be out of alignment

############################################

■Q3:XZ plane is my sketch plane, How to get the“perpendicular projection point” G of point K ? I can't do that by the snap tool or project tool. (the "S" shape curve is drawn in the ZY sketch plane )

############################################

■Q4:face A and face B and edge C are generated by a simple curve and the "Divide surface" command,

If I want to use the draft feature, it will not succeed. What is the reason for this failure?

I thought I was going to get this

But what I got is this actually

############################################

■Q5:How to convert the "offset of line_A" into a common or normal curve like an editable freehand curve?

############################################

■Q6:How to draw a freehand curve fitting the surface of the model?

The command under the"Style/curve/COS" only can draw on a single surface, it can not across adjacent surfaces.

############################################

■Q7:Under sketch mode, How to turn on the "extension-snap" of LINE_F to make the POINT_K pass through or make it align the extension?

############################################

■Q8:An old school problem, How to reduce the zoom speed(or zoom steps) when I zoom the view just using the mouse wheel? (I know shift+wheel or ctrl+MMB can help)

[Walker]

Correction of Q4 description:

Q4:face A and face D and edge C are generated by a simple curve and the "Divide surface" command

[tbraxton]

Q3 solution:

A sketch in the X-Z plane can use the point as a reference for point creation.

Creo 7 model for reference

[Walker]

Thank you for your guidance. But I still can't figure out the crucial step you get the position of PNT0 , what do you mean "use the point as a reference", I do want to use the upper-end point of the "S" curve as the reference point, but where is the "input port" where I can pass this point into the software as a reference?I tried the datum point which is outside of the "sketch creation" environment, I pick the upper-end point and the plane I want to project on, but it's not working

[tbraxton]

The point is projected onto the X-Z plane in feature sketch 3. Creo supports the creation of datum points within sketch mode. If you edit defintion of sketch 3 you will see it.

[Walker]

Yes, Creo supports the creation of datum points within sketch mode. But what I mean is I did see the resulting point which is datum point g (in your file it is PNT0), I see the result,  but I don't know the exact process you created it. Because Creo does not record that process in the file whether you created the PNT0 in sketch mode or not. If you create datum point PNT0 outside of sketch mode, it doesn't keep track of which reference objects you picked up. If you create datum point PNT0 within sketch mode, it's the same

[tbraxton]

@StephenW is quite right in suggesting a dedicated thread should be created for each of these questions. Create a new topic for Q3 and I will post a video showing how to create the point.

[Walker]

No problem, let me separate it.

[Walker]

The only way I found by myself just now is that create a datum axis first to tell Creo the "projection direction " of point_k, then get the cross point between the datum axis and the plane, So I don't know how you can create PNT0 more easily by avoiding these steps

[tbraxton]

Q4 The draft is applied to the solid face, not your divided surface. If you apply the draft to a surface (A) and not the face you will get your expected result. I am speculating on this as I do not have Creo 9 to test the divide surface function. In order to get the expected result on a solid face you would need to split the face, not the surface.

Model with surface draft used to create geometry for ref.

[Walker]

Thank you for your guidance. For Q4, I got exactly what you mean, thank you so much.

[StephenW]

From a solutions or searching standpoint, posting this many questions in one post makes it difficult for a "future user" to find an answer they have to one of your questions.

I would suggest that in the future, post each questions as a separate post. Then, as solutions emerge, you can mark the "solution". In the future, when another user is asking the same question, your solution will likely help them.

These are all great questions.

For the zoom, have you tried mouse settings for the zoom wheel? There are better mouse controls/drivers (other than the standard windows driver) that allow you to customize the mouse settings, even on a per software level, if you need more control.

[Walker]

Thank you for your guidance. I was worried about disturbing people with too many posts separately. I will separate my questions next time.

[kdirth]

Q2:  To create lines, create planes where you want the lines then use intersect between the planes and the surfaces.  Alternately you could project a sketch onto the surfaces.

Q5: My understanding of your request is a single, non-segmented, line.  Make a Copy-Approximate of the lines.  Select a line segment, Ctrl+C, Ctrl+V, Shift+select  remaining segments, change Curve type to Approximate.  If segments are all tangent, this will combine all into a single curve.

[Walker]

Sorry for the delay in my reply.Thank you for your guidance. But for Q5, I can only understand the green part of your reply, the rest is beyond my comprehension. Below is my corresponding understanding of what you mean, but I don't know what to do next. I would appreciate it if you could further explain the rest.🤝

[kdirth]

Looks like you are close.  Make the offset line lines first. Then use copy and paste approximate on the offset lines.  (Off setting an approximate curve will break the curve where it intersects a surface boundary.)  Ctrl+C (press and hold Ctrl key and press c) and Ctrl+V are old school shortcuts for copy and paste.  Non tangent lines will not copy as approximate.

Here is what it looks like in 7.0:

[Walker · Accepted solution]

I have broken down most of the questions in this post into separate posts for separation of concerns. Thank you all for your help. You can choose a place to help or browse solutions.