V-Carve Inlay Anyone?

[rlrhett]

Does anyone out there know how you would use F360 to create v-carve inlays?  For those who don't know, v-carve inlays take a positive relief and a negative relief cut with a v bit in contrasting materials.  The two are mated and one is cut or sanded away to reveal an inlay with perfectly sharp inside and outside corners.

This is a really great technique for decorative work because you don't need absolutely tiny bits to avoid rounded corners.

The Vectric software has built in scripts, but I assume it isn't too difficult to recreate the steps manually.  I'm more the artist than the computer guy so I'm having trouble thinking it through.  Logically it doesn't seem too complicated.  There are only a few things to keep in mind.  For eg. the positive shouldn't bottom out when mated so that you can be assured of a good fit.  Is there an evangelist out there who knows how this is done?  Here is there Youtube video on how Vectric has done it:

[HughesTooling]

The only thing I can think of is a program ZSurf, it will convert an image into a surface. See this thread for a bit more info. Other than that you could use Inkscape to trace the image then extrude in Fusion @PhilProcarioJr did a couple of screencasts a few weeks back, don't know if he can remember the thread.

Mark

[HughesTooling]

I found Phil's post, I bookmarked it as I thought it would be useful one day.

http://forums.autodesk.com/t5/design-validate-document/recommendations-on-how-to-super-empose-a-embl...

Mark

[michallach81]

Hi it's possible with engrave and pocket, only difference is that in Fusion we can't have pocket "inside" engrave, we need to do them separately. Because of that, it's not happening automatically and you need to find the offset for pocket (for 90 deg. chamfer mill offset will be same as depth).

In a short time I will make a screencast (no voice, cause I don't have mic at work), I will try to use same sizes for drawing, stock material and mills.

[PhilProcarioJr]

@rlrhett

What are you after for your end result? A model or actual machined part? For the model you can use the videos in the thread Mark posted to get all your lines from an image then you can use the video I posted here to V-Carve into a stock.

[michallach81]

@PhilProcarioJr

 It's impossible to mimic engrave in modeling, because engrave can create 3d path from random outline:

How you would guess that path to sweep? In a minute I'll post my vid.

[michallach81]

Here it is, as I said, I've tried to replicate same object as on video you've posted. Note that depth, tools and offsets will depend on job you have to do:

[michallach81]

I forgot to attach file, here it is:

[PhilProcarioJr]

@michallach81

Not sure why your getting those results...

[michallach81]

I know it's a bit tricky, if you would use tool bigger in diameter than overall width of closed path, engrave tool would find 3d path, of course if you will limit depth it will look as in your example.
Try to look closer in to how feathers are carved in that bird example (both my and a bird from vcrave).

[HughesTooling · Accepted solution]

Hi Michal, thanks for posting the screencast and file. I have a couple of suggestions to add and used your file in the screencast below.

The first is if you enable multiple depths in the 2d pocket op there's an option to add a wall taper so you don't need to do the math if you use a cutter with a different angle. You can set the max roughing depth to the total depth of cut and get one pass or less to get more passes. 

Second, if you unselect the outer profile and enable Stock Contours in the second setup, Pocket will clear the whole face.

Last If you use Create Derived Operation on the right click menu all your selections and setting are use. Fusion is real slow with those splines selected, not noticed that before.

Mark

[PhilProcarioJr]

@michallach81

I see what your saying and you can model that but it would be a tremendous amount of work that honestly wouldn't be worth it.

[PhilProcarioJr]

Just in case someone ever wants to model something like this....

[rlrhett]

I am sorry to everyone. I must have made a mistake in creating the original post. This was meant to be posted in the CAM sub-forum. The question is about machining an inlay, not simulating that in the modeling software.

To the moderators, can this post be transferred over to the correct sub-forum or should I simply re-post there?

[HughesTooling]

@rlrhett Have you watched the screencasts in post #7 & 11 they show how to machine and post 8 has a demo file. You import the file with New Design from file on the file menu.

Mark

[rlrhett]

Yes, you are right. I was so embarrassed that I posted in the wrong section (and that I saw someone had gone to all the trouble of posting a screencast of how to MODEL a cam operation) I had not seen the screen cast after post #5. #7 and #11 appear to be exactly what I was looking for.

Still, can this be transferred over to CAM subform so someone else interested might find it?

Thanks a million!

[HughesTooling]

@rlrhett if you need a post edited\moved click on report, bottom left of each post and ask the moderators to move the post.

Mark

[rlrhett]

I think the solution in #7 and refined in #11 works.  I'm trying to follow it, but I am not sure we took into account that for practical purposes the male and female can't be identical.  The male will likely bottom preventing a good mate.  Did that get addressed and I didn't see?

Here is a second Youtube of a different program's approach to this problem.  He calls the offset "Prismatic Overcut".  He addresses it @ 1:10, 4:26.

[HughesTooling]

You should get the same effect by moving the top face of the female side up above the level of the sketch. You will lose the sharp corners on the distance you move the face up but it probably only needs to be 0.02" to 0.03" so I doubt you'll notice with a V cutter.

Here's a screencast modifying the file above.

File's attached

Mark

[michallach81]

Hi guys, since yesterday you've posted several anwsers, and I will try to address them one after another, so please be paitient, and try to wait for all my 3 posts before you'll anwser. It may took me an hour.

First @PhilProcarioJr

 Phil, I know that we can create "fake" inlay that will look same as original, and under certain circumstances it will be the same, but with current tools and in this kernel (ASM) it's not possible to model what engrave tool is doing. Just take a look at how in theory it should be done , but Fusion kernel will not let us do that:

You can look for a workaround, but I have little hope for success.