Cut Option Unavailable in Revolve 230123

[pittsallen]

Hello Fusion 360 forum,

Base plate created and am working to place countersink holes in base plate.
Have locate two 6 mm holes 9 mm from base plate edge. 
Create plane perpendicular to face of base plate and created sketch
in plane. Drew right triangle in sketch and trying to revolve triangle

in base plate to make partial cone as countersink hole.
But when Revolve is selected the Cut option is not available.
The options available are New Body and New Component.

How to revolve triangles as partial cones in base plate body?

Thanks.

Allen Pitts

[davebYYPCU]

Place hole point centre, on the plate, dimension the centre points, use the Hole Tool, and select the fastener, is usually quicker.  Otherwise, 

Two things, the ok button is not ready, 

you have to select an axis, 

When the ok button is live, and you have selected the part of the profile that results in a cut, it will populate the dialogue box.

Might help.....

[jhackney1972 · Accepted solution]

You have a couple of sketches in your model that are not doing anything so I eliminated them.  You only really need one conical hole since they are symmetrical about the center of the plate.  Model is attached.

[pittsallen]

Hello @jhackney1972  , @davebYYPCU  and the Fusion 360 forum,

The replies by Jhackney1972 and davebYYPCU are appreciated.
Working to understand the process by which the model should
be created and Hackney's excellent video provides a lot of detail.
So went back to create model from scratch.

Base Plate w Countersink Holes
1. Create Component. Name Base Plate w Countersink Holes 230124
2. Create Sketch Name Base Plate
3. Select Center Rectangle tool. Make rectangle 74 x 74 mm
4. Create center PIR hole. Choose Circle Tool. Dia.: 24 mm
( I tried putting the countersink hole circle in the
Base Plate sketch but when the Base Plate sketch was extruded
it extruded the countersink hole circle as cylindrical
hole in the Base Plate. So I think the best practice would
be to extrude the Base Plate sketch and then create a
sketch for the countersink holes and revolve the countersink
holes as partial cones in the Base Plate.
4. Finish sketch.
5. Extrude sketch Extrude: One Side, Distance:3.2 mm, New Body, OK
6. Filet two outer corners 6 mm

7. Create Sketch. Name Countersink Holes. Select top face
of Base Plate for plane of Sketch.
8. Select Circle Tool. Make circle 6 mm.
9. Finish Sketch
Stuck now because I think the next step is to Project the
Countersink Holes Sketch onto the Base Plate Body but
when the CounterSink Holes Sketch is right clicked
the options are Create Selection Set, Offset Plane,
Slice Sketch, Save as DXF, Delete, Rename, Look At,
etc. but there is no Project option.

Perhaps the next step is not to project the sketch
on to the body.

Have tried right clicking on the Body to try projecting
that way but pretty much the same set of options appears,
no Project.

Tried going back into Edit Sketch mode but no change.

Is the next step to project the sketch onto the Body?
If so how to get the Project option to appear?

[laughingcreek]

I'm between screen cast tools right now, but hopefully @jhackney1972 is working on a vid for you.  conceptualy your not quite there on how to use project.  project works by projecting something from outside a sketch (another sketch object, a face, an edge, a body) INTO the sketch you are CURRENTLY editing.   There are sever projection types, they all come in handy, and if you are unfamiliar with them then I suggest you stop what your doing right now and go read up on them.  They're that important.  right up there with constraints.  essential for building parametric models.  you can find them here (while editing a sketch)-

[TrippyLighting]

To create contersunk, or counterbored holes we have a Hole tool:

[jhackney1972 · Accepted solution]

Here is a video creating your tapered hole using your original method which contains the Project command.  I then went back and created the hole using an extrusion with a taper.  This method involves a bit of Trig to find the taper angle which is ArcTan (3/6) if you are so inclined.  Model using your Revolve method is attached.

[davebYYPCU]

Side note, 

your comment between step 4 and the next step 4.

Extrude the circles but they are Cylindrical, unless

you call for a taper angle, then you can have the countersink angle cut, but you would have to know the taper angle. (Same single sketch)

More than a few ways to do it.

Might help....

[pittsallen]

Hello @jhackney1972 ,  @davebYYPCU , @laughingcreek  and the Fusion 360 forum,

Laughing's comment 'project works by projecting something from outside a sketch (another sketch object, a face, an edge, a body)
INTO the sketch you are CURRENTLY editing.' makes a lot of sense.

For instance, a clear implication is that one must be editing a sketch to project the geometry of another object
into the sketch which is being edited.

I believe what is neeed is for the geometry of the Base Plate to be projected into the Countersink Holes Sketch.
So the Countersink Holes Sketch. was place in edit mode.

And the Countersink Holes Sketch is right clicked and thes are the options available. Can'tBase Plate Body
seem to find 'Project/Include' ot 'Project'
.
So with Countersink Holes Sketch being edited a right click was done on the Bae Plate sketch. Options:

And so also the the Base Plate Body was right clicked. Options:

So apparently the model is some mode that prevents the 'Project/Include' ot 'Project' option available.

Have read several sections on Project and watch four videos on the subject. I think I need to know
what is the method or mode that is required for the model to be in for the Project option to
to appear. Didn't seem to get that info from these investigations.

Looking back at the screen shot in laughingcreek's post it is noticed that the Project option is
being accessed from the Create tab
So have updated process as follows:

Base Plate w Countersink Holes
1. Create Component. Name Base Plate w Countersink Holes 230124
2. Create Sketch Name Base Plate
3. Select Center Rectangle tool. Make rectangle 74 x 74 mm
4. Create center PIR hole. Choose Circle Tool. Dia.: 24 mm
( I tried putting the countersink hole circle in the
Base Plate sketch but when the Base Plate sketch was extruded
it extruded the countersink hole circle as cylindrical
hole in the Base Plate. So I think the best practice would
be to extrude the Base Plate sketch and then create a
sketch for the countersink holes and revolve the countersink
holes as partial cones in the Base Plate.
4. Finish sketch.
5. Extrude sketch Extrude: One Side, Distance:3.2 mm, New Body, OK
6. Filet two outer corners 6 mm
7. Create Sketch. Name Countersink Holes. Select top face
of Base Plate for plane of Sketch.
8. Select Circle Tool. Make circle 6 mm.
9. Finish Sketch
10. Edit Countersink Holes
11. Create > Project/Include > Include
12. Selection Filter: Specified Entities
13. Select all the lines and circles in the Base Plate Sketch
and click OK
14. Constrain the countersink circle to be horizontal
with Base Plate centerpoint.

From here tried using Create > Hole but that tool
does not seem capable of creating a simple partial
cone. So I think I need to do Revolve Cut.
But when I draw the triangle to be revolved
to do the cut it is being drawn in the plane
of the Base plate and and the cone is needed
perpendicular to the Base Plate so I think
I need to creat a plane perpendicular to the
Base Plate and then create a Cone Revolve Sketch in that plane
and plane a project geometry of the Base Plate Body
into the Cone Revolve Sketch

15. Construct > Offest Plane One of the planes
offered is thru the Base Plate center point so
the Z/X plane is selected.
16 Create > Sketch Name Cone Revolve Sketch
17. Create > Project/Include > Project
Selection Filter Selected Entities. Select
Sides and midpoints and countersink hole
centers. Click ok
18. Using Line Tool draft triangle describing
cone to be cut. Finish Sketch
19. Select triangle and select Revolve and the
Axis and click OK

The countersink hole is drawn correctly. (Yea.)

Now struggling with mirroring the countersink hole
to the other side of the Base Plate. Have reviewed
Hackney's excellent video but there is something
that needs to be chosen that is not being picked up.

Thanks.
Allen

[jhackney1972 · Accepted solution]

To mirror the Revolved tapered hole, select the Mirror command under Create.  Then change the Object Type, in the Mirror Dialog box, to Features.  Then select the Revolved tapered hole feature from the timeline.  Next make sure the Mirror Plane Select, in the dialog box, is blue and you will see the Origin pop up.  Select the origin plane you wish to mirror about.  You will see this done in the last video I uploaded.

[laughingcreek]

---

...
So with Countersink Holes Sketch being edited a right click was done on the Bae Plate sketch. Options:

And so also the the Base Plate Body was right clicked. Options:

So apparently the model is some mode that prevents the 'Project/Include' ot 'Project' option available...

---

I'm not sure why you keep right clicking on things expecting to find the project command.  project is a sketch command.  would you expect to find the LINE command or the CIRCLE command from a right click.  go to the sketch menu, its here-

[pittsallen]

Hello  @jhackney1972 ,  @laughingcreek , @davebYYPCU , @TrippyLighting and the Fusion 360 forum,

The replies are gratefully acknowledged. Progress is being made on
the journey from ignorance to knowledge.

A question if I may, directed at the reply from JHackney72 and the
excellent video marked Tapering Hole and Sketch.mp4 and
the resulting 
Base_Plate_w_Countersink_Holes_230124 - JRH.f3d
It was my conjecture that in order to create the right
triangle profile for revolution, a new plane, perpendicular to the
planes used for the Base Plate Sketch and the 
Countersink Holes Sketch would be required.
But in the video it seems the process was
simplified by not creating a plane in which
to create the sketch for the right triangle profile,
but by simply creating a sketch and projecting
the hole geometry from the Countersink Holes Sketch
into the newly created sketch.

But looking at the video and examining ....230124 - JRH.f3d
there is no third sketch.
So, if a new sketch was created to draw the profile in the
Z/Y plane, why is there no third sketch?
And if projecting is 'works by projecting something from outside a sketch (another sketch object, a face, an edge, a body) INTO the sketch you are CURRENTLY editing.' (thanks LaughingCreek) then how was the hole geometry from the Countersink Holes Sketch projected into itself?
I think I'm missing something. Like when you went into editing the Countersink Holes Sketch
you were able to grab a new plane or change the plane X/Y to Z/X. But if you were editing

the Countersink Holes Sketch how was the hole geometry projected into the Countersink Holes Sketch?
Thanks.
Allen Pitts




 

[laughingcreek]

In his video, John has the top level component active when he creates the sketch-

so the "third" sketch gets created at the top level, and can be found in the sketch folder at the top level-

so he projected the circle from the sketch "counter sunk holes" into the new sketch (located at the top level), creating the purple line.

[jhackney1972]

Thanks for catching and pointing out my error.  @pittsallen I apologize, I should have been more careful and activated the correct component so the sketch would fall underneath it. 

Edit: Attached is my corrected model.

[pittsallen]

Hello @jhackney1972  , @laughingcreek  and the Fusion 360 forum,

LaughingCreek: Thanks for helping me find the sketch. Was looking in the wrong Component.

Hackney: Finally figured out what the problem with doing the Mirror: The wrong mirror plane was selected.
It was thought that the mirror plane parallel to the axis where the features should be placed was to be selected.
I had to look at the video several times to realize the mirror plane being selected was perpendicular 
to the axis for placement.

Fault has been found for writing out long step-by-step instructions on how to model objects.  But
it has been found that
A. If the steps are written out they are better remembered.

B. Even then this seventy-two-year-old brain forgets an important click or dialogue box choice.
A written record has been more than once a savior.
Besides the steps are copied at the very end so if you don't want to read them just exit.
 Thanks

Allen

Base Plate w Countersink Holes
1. Create Component. Name Base Plate w Countersink Holes 230124
2. Create Sketch Name Base Plate. Choose the X/Y (flat) plane.
3. Select Center Rectangle tool. Make rectangle 74 x 74 mm
4. Create center PIR hole. Choose Circle Tool. Dia.: 24 mm
( I tried putting the countersink hole circle in the
Base Plate sketch but when the Base Plate sketch was extruded
it extruded the countersink hole circle as cylindrical
hole in the Base Plate. So I think the best practice would
be to extrude the Base Plate sketch and then create a
sketch for the countersink holes and revolve the countersink
holes as partial cones in the Base Plate.
4. Finish sketch.
5. Extrude sketch Extrude: One Side, Distance:3.2 mm, New Body, OK
6. Filet two outer corners 6 mm
7. Create Sketch. Name Countersink Holes. Select top face
of Base Plate for plane of Sketch.
8. Select Circle Tool. Make circle 6 mm.
9. Finish Sketch
10. Edit Countersink Holes
11. Create > Project/Include > Project
12. Selection Filter: Specified Entities
13. Select all the lines and circles in the Base Plate Sketch
and click OK
14. Constrain the countersink circle to be horizontal
with Base Plate centerpoint.

From here tried using Create > Hole but that tool
does not seem capable of creating a simple partial
cone. So I think I need to do Revolve Cut.
But when I draw the triangle to be revolved
to do the cut it is being drawn in the plane
of the Base plate and the cone is needed
perpendicular to the Base Plate so I think
I need to create a plane perpendicular to the
Base Plate and then create a Cone Revolve Sketch in that plane
and project geometry of the Base Plate Body
into the Cone Revolve Sketch
(Update 230125.
It was thought a plane needed to be constructed
perpendicular to the Base Plate and Countersink
Hole sketches to draw the triangle profile
so it could be revolved in the Base Plate
but Hackney showed that the plane could
be chosen when the Revolve Hole sketch
is created.)
15. Create Sketch. Name Revolve Hole
16. Project/Include > Project.    Project
6 mm hole geometry from the Countersink hole Sketch
into the Revolve Hole sketch. Selection Filter Selected Entities.
Select the countersink hole centerpoints. Click ok
17. In the Sketch Palette click Slice so the
circle geometry can be better seen.
Using the line tool draw the triangle
beginning at the hole centerpoint down 6 mm
back to the edge of the circle and back over to the
countersink hole centerpoint. Finish Sketch.
18. Select Revolve, select the
triangle profile and the Axis. Make operation Cut.
and click OK
The countersink hole is drawn correctly. (Yea.)
20. Mirror: With the Base Plate Body selected, choose
Mirror from the Create tab. Object Type: Feature
Object: Select the cone hole feature . Turn on the Base
Plate Component Origin Point. For Mirror
Plane select the Z/Y plane. Compute Type: Adjust
The new cone hole appears as preview. Click OK

The cone hole can also be profiled without
drawing the triangle profile in the Revolve
Hole Sketch making the Revolve Hole sketch
obviated.
The Base Plate Body is selected and Extrude tool is
chosen. The selected cone hole profile is selected
the Distance is input as -6mm The Taper
Angle is input as the arctan of the side (6 mm)
and base of the triangle  or 26.57 degrees.
ArcTan = 3/6 = 26.57 degrees.

As is almost always the case in Fusion 360
there is more than one way to skin the cat.

Peace. Out.