Engraving with pocket, 2 different chamfers

[Anonymous]

Hi,

I have multiple related questions, but I'll try to keep everything as concise as possible. Basically, I'd like to create a chamfered pocket in a certain shape; as an example I've used an M-like shape which has 1 concave corner, as well as both 90 and 45 degree convex corners. I use a 200x200x10mm stock and the depth of the extrusion is 5mm.

In my view, there seem to be 2 ways to create a 45 degree chamfered pocket in the correct shape, which I'll try to explain:

Model A: extrude the shape 5mm down and create a 45 degree draft on the sides. This is basically the same as adding a 5mm chamfer instead of a draft, or if you'd use the offset tool when sketching. The concave corner will still be a sharp corner in the "inside shape". However, when CAM engraving the edge, I've noticed it creates a different shape, which was a bit more complicated to model:

Model B: in the sketch, create a 5mm offset on the inside of the shape. Add a 5mm fillet to any concave corner. Extrude the inner shape 5mm down, and then cut out a loft from the extruded pocket to the outer shape. This creates a similar shape to using the engrave tool. For any concave corners, the "inside shape" will have an arc.

So those are 2 slightly different implementations of the same idea. See my attachment for the file.

Question 1: is this the right way to model these bodies? Is there an easier way to get to Model B? (I know this is technically a design question, not CAM, but hope you can answer here as it's related to the rest).

Then I've tried to mill both designs, using only a 5mm flat endmill and a 25mm 90° spot drill.

For Model A I've used a pocket operation with the flat endmill on the inner/lower surface. The I've used a trace (with the spot drill) to follow the contour of the inner surface. I could not use an engrave operation on the outer contour, or it would cut the concave corner too short (like Model B). This left me with rounded corners, so I've used another trace operation (again with the spot drill) on the diagonal corner lines of the 4 convex corners. Selecting these lines added some additional horizontal lines as well, as I was unable to select just the diagonal slopes. The final simulation looks OK, except for some tiny leftover pyramids in the convex corners where the flat endmill could not reach. I'm unable to pocket this out with the spot drill.

Question 2: how to mill Model A? Is this the right way? How to get rid of the leftover stuff in the convex corners?

For Model B I've again used a pocket operation with the flat endmill on the inner/lower surface. Then I've used an engrave operation with the spot drill (but only to a depth of -5mm), which also took care of the convex corners, so no need for an additional trace on the diagonal corner lines. The final simulation is similar to my result of Model A: looks OK, except for some leftover bits in the convex corners.

Question 3: how to mill Model B? Is this the right way? How to get rid of the leftover stuff in the convex corners?

My attempted milling setups are included in the attachment as well.

Finally, I was trying to do these things with a smaller V-bit, let's say a 5mm 90° spot drill. I ended up using offset planes to make intersection sketches partially down on the extrude (say -2mm and -4mm). Then I've added additional trace (Model A) or engrave (Model B) operations on those outlines to clean off the entire chamfer. For Model B, I've tried using the engrave with the smaller bit on the outer outline and setting the bottom height to -5mm, but along the straight edges it doesn't clear the top, it basically traces the lower (5mm) outline and only comes up in the corners.

Question 4: how to use a smaller V-bit? Is there something like a step-down which goes down the slope? Manually creating multiple passes at different intersections is very tedious.

As a final note, I'd like to say all of this was very easy when I've used Estlcam, using only a single operation, and even supporting smaller bits. It would go up into the corners to create sharp corners (similar to what Fusion CAM engrave does), go down the chamfer in multiple passes (if using a small bit) and even clear the entire pocket using the V-bit, leaving no "corner pyramids". Of course, clearing out a large pocket with just the tip of a V-bit is not ideal and does not leave a nice surface finish, but at least it clears the corners.

Any help / advise is very much appreciated. Thanks in advance!

[daniel_lyall]

What you are try to do is a inverted prism, what can be done with a few tool paths and some well placed sketches.

Basically have a toolpath to cut the bottom flat then use a traces, project, contour or the engrave toolpath (what is a V carve toolpath) one of these 4 can/could do what is needed.

You have a offset sketch for the bottom and the toolpath to cut the angled sides basically a offset in of what you wont to do.

Use a endmill to cut to the bottom depth and a Vcarve engrave to cut the angle sides.

[daniel_lyall]

Most of what you have done already is fine, you just need to play with the settings to get the angles correct use sketches to change the path.

One thing that helps is the tool size and angle, you have the tool the same angle and the tool width the same as the depth. 5 mm depth = 10 mm tool.

Moving the bottom height helps to.

[Anonymous]

Hi Daniel, thank you for your reply. It's actually not a prism (what geometric shape is an inverted prism?) because of the chamfered edges. If you read my text (sorry it's a bit long), you'll see that I did just what you described (flat endmill pocket + trace/engrave), but it won't do. First of all, Model A can't be done with engrave, because it would cut the inner concave corner short. Second of all, you'll still end up with some leftovers. Please see the attached file for both models and toolpaths.

[Anonymous]

---

My previous message was a reply to your first, did not see your latest message yet.

I'm not sure what you mean by "use sketches to change the path". Don't I already have the correct sketches?

As for the tool, I'm already using the right angle tool (90° which gives a 45° chamfer) and using a large size to have at least 5mm for the chamfer. If I select a 10mm bit, the default bottom height will not be enough (only 4.75mm). I use an extremely large one so I will definitely have enough, but see my last question for how to use smaller ones.

I do use bottom height, set to 5mm so the large bit does not go all the way through. What do you mean by moving it? I can't move it, because I need just 5mm depth.

[daniel_lyall]

Inverted prism toolpath ( it's a tool path name). Yer I looked at your file you have to adjust the settings to get it to cut how you wont or use sketches and adjust settings.

You have to match the tool to the toolpath, sharper the corners are, the smaller the tool you have to use to get it to fit where you wont to stick it.

There are other programs that are click and go I have a few that are like that what do this sort of thing with ease.

[Anonymous]

---

@daniel_lyall wrote:

Inverted prism toolpath ( it's a tool path name). Yer I looked at your file you have to adjust the settings to get it to cut how you wont or use sketches and adjust settings.

You have to match the tool to the toolpath, sharper the corners are, the smaller the tool you have to use to get it to fit where you wont to stick it.

There are other programs that are click and go I have a few that are like that what do this sort of thing with ease.

---

I'm sorry, but "you have to adjust the settings" isn't very helpful to me.

About the tool: a smaller or larger V-bit still has pretty much the same (pointy) tip, so it won't do much difference. As long as it's large enough to reach the full chamfered walls, the results are exactly the same.

Of course, the flat endmill could be smaller, but it will never be able get into the corner that the V-bit made (either by trace or engrave). That's why I was asking how to let the V-bit take this out using a small stepover, which Fusion won't let me do (tool cannot be used for this).

[daniel_lyall]

I am replying based on what i have found to work in fusion, doing v cave type toolpaths. 

Link to fusions learning section on cam toolpath tabs 

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID19769567-5A74-4630-B8D4-9995FFAC5611

 You can use sketches in fusions cam for toolpaths.

Doing a offset sketch from the top edge out by 5 mm and useing this as a toolpath, lands the tip of the v bit on the bottom of the angle, if it is going to deep lift the bottom height up to -5 mm.

[HughesTooling]

Sorry haven't read all the posts but I'd not bother modeling the chamfer at all. Take a look at the attached file, I've used the taper option in pocket to get the offset at the bottom face. Note to make taper work in pocket and 2d contour the top height needs to be Selected Contours and the bottom needs to be Selected Contours minus the depth, so both need to reference the Selected Contours in both heights. Using pocket like this you can even rough at different levels like 1.25mm and the taper will be correct.

Mark

[HughesTooling]

Just in case you want the A version with all sharp corners here's a way to select the edges to give a bit more efficient tool path. Note Alt will allow a single segment selection.

Mark

[Anonymous]

---

@HughesTooling wrote:

Sorry haven't read all the posts but I'd not bother modeling the chamfer at all. Take a look at the attached file, I've used the taper option in pocket to get the offset at the bottom face. Note to make taper work in pocket and 2d contour the top height needs to be Selected Contours and the bottom needs to be Selected Contours minus the depth, so both need to reference the Selected Contours in both heights. Using pocket like this you can even rough at different levels like 1.25mm and the taper will be correct.

Mark

---

Wow, this "Wall Taper Angle" setting is great! Did not know about this. Perhaps because it's a bit hidden away in the "Multiple Depths" parameters.

It's working for me even with other references (e.g. "Stock top"), so I'm not sure what you mean by both top and bottom height needing to reference "Selected contour(s)". I'll keep it in mind in case I ever run into issues.

Thank you @HughesTooling for taking the time to make a file for me. I've got 2 questions:

- I noticed you used a Boundary Fill to duplicate the body. Any reason for this? What are the advantages to other methods? Like for example the Move tool with "Create Copy" checked?

- After running a simulation of your ModelC setup, I still see similar leftover bits in the outer corners, where the V-bit went into the sharp corner, but the flat endmill could not get into the corner all the way because of it's diameter. I ran into this same problem. Would be nice if the spot drill could also be used for pocketing, perhaps with Rest Machine enabled so it would only need to do these corners. Could this be solved by defining a custom tool?

[Anonymous]

---

@HughesTooling wrote:

Just in case you want the A version with all sharp corners here's a way to select the edges to give a bit more efficient tool path. Note Alt will allow a single segment selection.

---

Just what I needed, that Alt trick! I was already wondering why it would always select additional (seemingly random) segments together with the one I clicked. You even combined the 2 trace operations into 1, nice idea.

[HughesTooling]

---

@Anonymous wrote:

---

@HughesTooling wrote:

Sorry haven't read all the posts but I'd not bother modeling the chamfer at all. Take a look at the attached file, I've used the taper option in pocket to get the offset at the bottom face. Note to make taper work in pocket and 2d contour the top height needs to be Selected Contours and the bottom needs to be Selected Contours minus the depth, so both need to reference the Selected Contours in both heights. Using pocket like this you can even rough at different levels like 1.25mm and the taper will be correct.

Mark

---

- I noticed you used a Boundary Fill to duplicate the body. Any reason for this? What are the advantages to other methods? Like for example the Move tool with "Create Copy" checked?

I'll have a look at the corner problem tomorrow but I'll answer the boundary fill question. The problem with copy is a big edit to the model can break the copy and there's no way to fix or reselect. If you ever run into this problem the only fix is delete the copy which can snowball through your timeline breaking other features and become a nightmare to fix. With boundary fill you can just reselect, you can even select a different body if you need to.

Mark