hole starting on rounded surface?

[Anonymous]

Hi,

I have a body (base cube) with one face rounded. On the opposite side of the rounded face, at precise coordinates (10x10 - for example), I want to have a conterbore hole come though - meaning I want the hole to end there.

I couldn't figure out how to create the hole starting on the rounded face.

One solution I thought of was: create an offset plane from the non-rounded face, and position it at the max of the curvature. Then create a sketch on the plane and place a circle where I want the hole to start. This approach seemed to have worked, but doesn't parametrize well - the offset plane is not 'attached' to the body. So if I'm moving or scaling the body, the offset plane and attached sketch do not move.

Any ideas on creating a hole like this?

Thank you!

[Anonymous]

Hi, I would do it by creating a sketch point on the curved surface and dimensioning it at precisely the right location.  Then using Create > Hole or draw circle at that point on Tangent at Point construction plane, and extrude a cutting cylinder from that circle. This video shows a similar workflow, and depending on your surface (cylindrical or spherical curve) will get a line or point from Intersect command of the curved surface in Sketch mode:

https://www.youtube.com/watch?t=149&v=HvOV38d8JIo

Let me know if you need more help.

Good luck!

Jesse

[Anonymous]

Thank you Jesse, I really appreciate your reply.

Just tried something like you described but didn't have any success.

I attached a few screenshots with my setup. In sketch_constrains image, the circle is where I want the counterbore hole to end.

Disclamer 🙂 - total CAD noob here and just got my hands on Fusion last week.

[Anonymous · Accepted solution]

Well there's several ways to go about this, probably what I would do is the following.  First create a sketch on the flat face of the object like you did, and only place a point representing center of hole and dimension it to the two edges like you did.  Then stop that sketch and create a new sketch (this is required), and be sure this second sketch is also defined/made on that same back flat face of the object, then go to Sketch > Project/Include > Project to surface, for the Faces choose the rounded face, and for Curves choose the point you made in the previous sketch.  Also for Project Type choose Along Vector, and that will cause projection along vector direction that is perpendicular/normal to sketch plane of previous sketch you made containing the hole centerpoint.  You can see below how a new point will be created on the curved surface. 

Now to use the Hole tool under Create, will need to use it twice, so one option is under Modify > Parameters to create a user defined parameter, here I call it counterdiam.

Then in both Hole operations, I type counterdiam for the counterbore diameter (note first Hole operation I have as just Simple for Hole Type -- the purpose for this first Hole operation is to remove the small amount of material above the plane containing the projected point...note to get Hole tool going in right direction, may need to press the Flip Direction button). 

Alternatively can just note the parameter name for the first Hole diameter, here it says it's d4.

Then in second Hole operation (note the second sketch visibility will be turned off after first Hole, so need to turn sketch visibility back on), for the counterbore diameter I type d4 to correspond to previous hole operation, and now I also choose Counterbore option. 

When you move the original point you made representing the hole center, all this will parametrically update. 

Note when you do the Hole operations, the hole axis will be created perpendicular to to sketch plane that was defined by the sketch that contains the projected point, hence the importance of defining that second sketch on the proper back face. 

Let me know if you have any other questions (and check hobbymate.net soon for a library of interactive learning content for Fusion 360).

Jesse

[Maowen_Zhang]

Great idea using project curve to surface to achieve this! 

[JamieGilchrist]

hi wvrius,

I think Jesse's suggestion and approach is a good one, albeit somewhat advanced for a "noob", but it nicely illustrates the power of parameters.

The nice thing about any CAD system is there are always multiple ways to achieve what you are trying to do and the more experience you have with them the more effecient of a modeler you'll become, don't be afraid to try different approaches.

So I wanted to go back to your original method.

"One solution I thought of was: create an offset plane from the non-rounded face, and position it at the max of the curvature. Then create a sketch on the plane and place a circle where I want the hole to start. This approach seemed to have worked, but doesn't parametrize well - the offset plane is not 'attached' to the body. So if I'm moving or scaling the body, the offset plane and attached sketch do not move."

Your thinking on this was right, but the tools didn't quite match what you were expecting, so I wanted to show you an alternative that would work the way you were describing or at least expecting.

In three easy steps I was able to create the scenario you described above, and this could have been done in two step, but I wanted to illustrate how construction planes can work for you.

after createing my base shape;

1.  create a mid plane construction plane, select the two outer parallel faces. once the center plane is created if you update the main shape by editing the sketch, the plane will stay centered to the geometry. 

Note: this is the step you could eliminate if you built your sketch for your base feature centered around an origin plane, that way an origin plane is always at the center of your design.

2.  create a sketch on the midplane, use project and select the face of the arched end of your model.  This creates the points at the extent of your arch and parallel to the two sides.

3.  create a tangent to face through point construction plane, select the arched face and the point at the end of the sketch

Now as you change the parameter of your first sketch, the construction planes will update as you expect, keeping that tangent plane "attached" to the body.

remember this is just one approach to getting the results you want and this particular approach helps ilustrate how construction geometry ties to the model.  YOu could get here in one feature using the tangent plane construction plane (as apposed to the Tangent Through Point above), but you'll need to do some fine tuning to get the precise result you want.

hope this helps and I'll post some models later today to share with you showing a couple different aproaches.

[JamieGilchrist]

Here are three different examples of achieving the same result, just a little different approaches.

when you open up the models take a look at how the construction planes stay linked or attached to the body as you adjust the original sketch.

hint you can turn on the visibility of the sketch and grab an edge and drag without having to go into the edit sketch environment.

enjoy.

[Anonymous]

This is perfect, exacly what I was trying to achive.

I did try projecting initially, but I didn't know that I have to create a secondary sketch for the projection to work ... still learning my way through it.

Thank you very much.

[Anonymous]

Hi gilchrj,

I really appreciate taking the time to answer. Your reply and examples on how to make contruction planes stay linked to the body were extremly helpful.

Thank you!

[Anonymous]

Great!  Have a great time learning, and be sure to post any other questions that come up. 

Jesse

[JamieGilchrist]

no problem. And like jjurban55 says post any other questions that come up. The fusion community, both our users and Autodesk employees are really helpful and eager to help new users get un-stuck.