v-carving/embossing

[denver]

Hello,

I sometimes get orders to carve wood type, for letterpress printing. I've been using a different software product to prepare the toolpaths for those orders, but I would like to switch to VM. I have two difficulties with the old software that I'm hoping VM will overcome:
1. The old software uses the v-bit to clean up material left by the flat tool, so there's always a trade-off between the size of the clearance tool and the time spent v-carving. Larger tools remove the material faster, but leave more behind for the v-bit to clean up.
2. The old software has the two operations closely linked, so if I want a second pass with the v-bit that runs just around the edges, I have to jump through some hoops to do that.

I've been looking at how VM does v-carving, and I have two related questions:
1. Is there a way to specify a re-machining operation after the initial v-carve roughing operations? This would let me use a fairly large end mill to clear most of the material away, followed by a smaller one to help clean inside corners. I haven't found a way to do this, but hopefully someone can suggest something.
2. In order to avoid any uncut material that extends to the surface, the final roughing pass needs to be done with a tool whose radius is less than the distance to the v-bit center at the material surface. For example, the center of a 60 degree v-bit is about 0.058" from the edge when cutting 0.1" deep.Therefore, a bit with a radius of less than 0.058" would be necessary to avoid any uncut material. Is this correct? If it is, then a re-machining operation would really be helpful.

Otherwise, it looks like VM would be an excellent replacement for the software I'm currently using.

Regards,

Denver

[MecSoft Support]

1. You would have to generate a 2nd v-carve roughing toolpath using a smaller diameter end mill to remove any uncut material being left by the larger tool. This might end up cutting some air.
The other alternative would be to generate a 3 axis Horizontal Roughing & Re-Roughing operation using end mills. The re-roughing operation is used to create toolpaths in areas that were not machined by previous operations. Unmachined areas are determined by comparing the part to the stock remaining after the previous operation. For this you would have to create a 3d model the part geometry.

2. Remachining operation only takes into account the reference tool diameter of the previous cutter. Currently we do not have an option to specify the taper angle along with the reference tool diameter.
We will add this to our enhancement requests to be able to specify taper angle along with the reference diameter for re-machining operation.

Hope this helps.

[denver]

Thanks for the response.

Making a 3D model of the job is an interesting idea, but probably not practical most of the time. A single order can involve several hundred individual pieces of type. But I will keep it in mind for the smaller orders.

I tried creating a second v-carve roughing operation with a smaller end mill, but since it doesn't know anything about what was done with the larger one, there really is a lot of air cutting. At that rate I might as well simply use the smaller tool for the whole job. I was hoping for a way to clear most of the material with a larger tool, then concentrate on the tight spots with a smaller one.

I've also tried the 2.5 axis re-machining operation, but as you point out, there's currently no way to tell it about the taper of the final tool. Being able to do that would certainly help. Thanks for adding that to the list.

However, there are often going to be areas too small for the end mill to get at, but still large enough to cause trouble. It would also be helpful to be able to clean those areas up with the v-bit.

Thanks again,

Denver