component positioning with sketches

[alexanderhermann83]

Hi there,

I'm new in Fusion 360 an used CATIA V5 for 10 years and now I wan't to try out the fusion.

I'm designing cutting tools and want to position cutting insert with 3 sketches.

One sketch is for axial angle, one for radial angle and one for the insert type and rotation around the Z Axis ( I use Z up  as default modeling orientation)

The first two sketches are just lines with angles, I create a plane with this two lines and create a third sketch on this new plane with the profile of the cutting edge (in this example a 80° insert with 0.8mm corner radius)

Now I tried to position the cutting insert with this third sketch, therefor I tried to make joints but without success.

Could you tell me how I can position the cutting inset? The goal is to have a parametric assembly where I can change the 3 angles, axial , radial and the rotation around Z

The design method works stable in CATIA V5 and now I want to know if I can adopt it to Fusion 360 or do I have to use another method?

Kind regards

[etfrench]

Can you attach your file to the thread?  It would make it easier to see your workflow.

[alexanderhermann83]

Here is the link:

https://a360.co/2vb3jtQ

If this is not enough I browsed a file below.

Please tell me if the link was enough.

[davebYYPCU]

Fusion Joints are different to other systems.

Your pics make it had to read, 

You only need one joint, with angles and offsets, if I have got what you are after, 

To use a Joint in a Sketch, you can snap to end, (midpoints, in my case) or offset the Joint origin to other locations, for the needed flexibility. This pic has an inclined plane in two directions, on a 3d line, with a Joint origin snapped to the midpoint of the line, (for demo purposes. Component 1.)

The plane (Component 2) was constructed as a Plane on a path, to simulate the base face of the insert.

You would joint the base face of the insert on the axis of the bolt hole, with the 3d line Joint origin in Component 1, any height (offset) from the origin, and any angle (rotated) around the origin, at the time of making the Joint.

So in this pic, you can drag (3d Move) the open end point of the blue line, and the face of the insert would remain perpendicular to the origin point.

Again I am not so sure I am on the right track.

Might help....

[davebYYPCU]

The file loaded locally, 

Skeleton needed a line to the centre of the insert, on it's alignment plane sketch.

Joint Origin, at the end point.

Rigid Joint to the end of the line from the centre of the Insert.

Might help....

[alexanderhermann83]

Thanks for your fast support, I will check your download later that day and see if this is the solution

[alexanderhermann83]

The Insert is rigid now, but it stays on the same place when I change the sketches axial and radial.

So the design is not parametrical. If I understand right I have to put all parameters as I'm creating a joint. How can I control the parameters? Or is there a different method to position a component beside joints?

[davebYYPCU]

Two things, I am having a hard time visualising the problem, without being critical, I will put it this way, 

I am used to seeing your inserts bolted to a toolholder.

you appear to be designing a home made toolholder, which is fine.

the parameters to fix the insert, belong in the toolholder, not the insert.

As far as I remember, (not at the desktop yet) the skeleton component, or its parent is grounded, you can’t move the toolholder if it is grounded, but you can still parametrise the toolholder shape / features.

Might help....

[davebYYPCU · Accepted solution]

Ok, I have got your parameters working, presuming you still have my file, 

To make my headache go away, I rotated the body in the Insert, 40 degrees, so the origin in the insert is now aligned with the nose of the tip radius.  (When making the Joint you could do the rotate 40 degrees there.)

Edit sketch 9 - Project the moving line in the angle parameter, from Radial and Axial sketches.

Make my centre line with the joint origin on it, symmetric with the two projected lines.

Edit the Joint Origin to align with the centre line. (45 degrees)

Probably not right with draft angles and stuff,  but it is working.

[alexanderhermann83]

Hi davebYYPCU, sorry for the late reply and I didn't want to make you a headache.

I finished some more exercises from "Getting Started with Fusion 360 Tutorials" to better understand the behavior of joints. I understand now that every component needs only one joint to be fully defined (please correct me if I'm wrong).

There are some strange behaviors that I have to get used to for example: I cant take the axis of the axis system in a sketch to make a dimension it creates always a construction line that I see when I'm leaving the sketch. That makes it a bit confusing when I have a sketch with 1°or 2° then I see 2 lines very close to each other. Is there a possibility to hide this construction lines? Another one is that I can't dimension 0° in the sketch, do I have to switch to horizontal or vertical constrain or is there a way to make the 0°?

[TrippyLighting]

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@alexanderhermann83 wrote:

=Another one is that I can't dimension 0° in the sketch, do I have to switch to horizontal or vertical constrain or is there a way to make the 0°?

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YOu'll have to apply a horizontal vertical constraint.

However, I do agree that it would be very nice if the angle could be 0 degrees.

[alexanderhermann83]

I found a solution for 0°, If you go to parameters table then you can type 0° and it works