Fusion
Community
Hello,
Bear with me since this is my first post after doing some research and stuck on why is this happening. I've got myself into CNC as a hobby with my first machine and using Fusion 360 as a start. I've done tutorials and some you tubes and this still perplexes me for some reason.
My test on the wooden board is a cut of -2mm cut depth in 'Z' but once I configure the file and post process it gives me a depth of -9.444 cut without understanding why it's doing that. The trace works perfectly as it should.
(20240523-20d3mm-wedding-engrave-03)
(Machine)
( vendor: Sainsmart)
( model: Genmitsu Reno-4040)
( description: Generic 3-axis)
(T1 D=3.175 CR=0 TAPER=10deg - ZMIN=-9.444 - chamfer mill)
(***THIS FILE DOES NOT CONTAIN NC CODE***)
(When using Fusion for Personal Use, the feedrate of rapid)
(moves is reduced to match the feedrate of cutting moves,)
(which can increase machining time. Unrestricted rapid moves)
(are available with a Fusion Subscription.)
Every engrave has a larger cut depth than the original cut design; still unable to come to terms what could be causing it. The tool i'm using is a genmitsu Vshape V20 series 1/8 shank with 30mm overall length.
I tried to use 'sketch' as part of engrave and it still gave me -9.444 depth cut instead of -2 cut depth.
I think I might have found the solution by coincidence; yet to be verified on CNC machine.
For some reason when checking the 'heights' on the engrave setup the 'bottom height' was -8.23
for some odd reason it totalled up to -9.444 in z cut depth. but when I changed the 'bottom height' from the number to 0 cut depth
the final post process file gave me
(T1 D=3.175 CR=0 TAPER=10deg - ZMIN=-2 - chamfer mill)
Now I need to test this out on CNC.
My question is, where did the bottom height offset got the numbers?
Can you export the design as an F3D and share here?
The depth is calculated off the cutter diameter and angle, so max depth the cutter can cut the angle. As you are using Engrave it will only cut to the point where there are 2 points of contact in the area being cut, so for small letters it'll never cut to that depth. You can still set a max depth from the top height so the Engrave will still maintain 2 points of contact, either between 2 sides of the profile or one side of the profile and the depth you set. If you share the design it'll be easier to demonstrate.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@trojanowski_d wrote:
Every engrave has a larger cut depth than the original cut design; still unable to come to terms what could be causing it. The tool i'm using is a genmitsu Vshape V20 series 1/8 shank with 30mm overall length.
Engrave like most of the 2d machining ops is not model aware so you need the set the max depth manually.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
So here are the two files with two version v4 is the unmodified bottom height and v5 is the modified bottom height to 0 mm.
- wedding v4 - has unmodified depth but creates a single line engraving, however the cut depth jams the spindle (75W) with a 70V20 version genmitsu tool for carving (3.175mm 20 degree carve
- wedding v5 - has a modified height to 0 bottom height but creates a dual line for engraving like tracing mode. see picture results. I'm trying figure out the correct depth to carve a single line without jamming the spindle. since the original cut depth of letters is 2 mm.
it's on a plywood 12'x12' and 1/4' deep. (305mm x 305mm x 6.35mm)
I like the trace work but lettering I'd wish it would come out as a single engrave line not traced.
To get Engrave to create a V carve effect you should select the contours at the top face then set the max depth on the depth tab.
So select contours top face.
Set depth to -2mm.
Also for the size and shape of these letters you will get a better effect with a 60° cutter.
This will work well for all of the text. What do you want for the man and woman? Do you want to pocket the whole area then pick out the fine details with engrave? You can use pocketing with flat bottom cutters the finish with one of the taper cutters using engrave.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
