Modeling question

[zaxis]

I need some advice to carve a decorative lid on a 10 x 7 ornamental box. I want to use the border clip art "rope" I think I need to get the corner clip art for that as well....not sure. With this design around the perimeter of the lid I am trying to give it the raised panel effect in the middle. This would require using a bevel. The rope and the center of the lid need to be the same height. I'm sure its not that complicated but I can't seem to make it work.

[SteveNelson46]

Something like this? You already have Aspire so making the rope border yourself is the key. I used the Extrude Along a Centerline tool and the rope link clipart.The center is created with a moulding toolpath. Let me know if you want the example file. It's not a finished project and still needs some work but it illustrates the process I used.

[zaxis]

That’s pretty close to what I am trying to do. Your file would be a good learning tool if you wouldn’t mind. Thanks for your reply.

[SteveNelson46]

Sure. Here's the link to download it. It's not a finished model and will probably need some touch-up.

https://drive.google.com/file/d/1jticCO ... sp=sharing

[zaxis]

Is the extrude a separate piece and just added to the rope extrude??

[SteveNelson46]

I put the rope link on the page, reduced the size about 25 percent, rotated it about 10 or 15 degrees and set it to merged. Then I used it as a component in the Extrude and Weave tool. See the attached settings in the pic of my last post. Then I created a vector boundary around the rope component and used the inside and outside vectors to limit the 3D toolpath. The Moulding toolpath is a separate process. I had to play with the size of the drive rail (rectangle) a little to match the inside of the rope component. The profile is just a slanted line to get the slope around the perimeter.

[BrooksM]

Greetings

Michael Mezalick has a couple great tutorials going into depth creating rope or chain link borders:
3D Modeling for Newbies Lesson 6 Extrude and Weave Part 1 & 2



Good Luck
Brooks

[zaxis]

Thanks a lot for your help. Much appreciated

[zaxis]

More questions about modeling toolpaths. I am not new to CNC but I have not done much real carving with mine so I have some probably really stupid questions. So as I am understanding it the roughing tool path is usually done with a .25 endmill. The machining allowance is critical because the finish tool path is done with a ball nose and the depth of cut of the ball nose is going to take is whatever is left with the machining allowance. If you leave too much the ball nose will be taking too much of a cut and risk of breaking. Am I understanding that right. If I leave a machining allowance of .04 then that is what the finish cut will take with the ball nose and I have no control over setting the depth of cut??

[zaxis]

Another thing......carving Cherry, using a .125 3 flute ball nose. leaving a .04 allowance what is a good starting point for speed and stepover? 100IPM and 3% stepover seems to take way to long to complete the job so It must be wrong

[ZipperHead55]

Another thing......carving Cherry, using a .125 3 flute ball nose. leaving a .04 allowance what is a good starting point for speed and stepover? 100IPM and 3% stepover seems to take way to long to complete the job so It must be wrong

If you are talking about the roughing toolpath, 3% is WAY too low. I use a 1/4" ball nose, and have 41% for my stepover, and 100IPM (I have Axiom AR4Pro as well). For finishing I use 1/32" r and 1/64"r at 150IPM and 7-8% stepover. I would recommend getting a larger ball nose (ie 1/4"), since you'll be able to run it faster than a 1/8" (.125") bit.

Allan

[zaxis]

Great...Thanks for the reply. I know there are no set numbers for this but at least it is a starting point. Am I right about the allowance? There is no depth setting on the finish ball nose. It just removes what is left?

[Adrian]

So as I am understanding it the roughing tool path is usually done with a .25 endmill. The machining allowance is critical because the finish tool path is done with a ball nose and the depth of cut of the ball nose is going to take is whatever is left with the machining allowance. If you leave too much the ball nose will be taking too much of a cut and risk of breaking. Am I understanding that right. If I leave a machining allowance of .04 then that is what the finish cut will take with the ball nose and I have no control over setting the depth of cut??

Another thing......carving Cherry, using a .125 3 flute ball nose. leaving a .04 allowance what is a good starting point for speed and stepover? 100IPM and 3% stepover seems to take way to long to complete the job so It must be wrong

Depends on the size of the job but a 1/4" endmill for roughing (40% stepover) and a 1/8" ballnose (8 to 10%) stepover is typical. Feed rate wise you'll probably never get close to the programmed feed rate unless you've set it extremely low as there is so much combined horizontal/vertical movement. Overall movement speed is constrained by the z axis.

Yes there is no direct control over the finishing pass cut depth. It will cut as deep as it needs to in one go which is a good reason for not using a roughing tool that is too much bigger than the finishing tool otherwise there are likely to be deep areas that the roughing tool didn't reach that the more delicate finishing tool will plunge right into.

[zaxis]

Thank you Adrian I appreciate your reply

[zaxis]

Thanks to all of your advice and help my plans are turning out for the most part pretty well. I have successfully created what I have dreamed up for a decorative box. I was able to carve out a ogee shape for the sides and project a vcarve design onto its surface. When I did my 3d roughing pass I used a 1/4 endmill and used a 1/4 offset around the perimiter. That seemed to work just fine as it let the tapered ball nose cut down as it needed without the side rubbing. My question is about the finish cuts with the tapered ball nose. I chose to use a .25 tapered ball nose to finish with. I also programmed a offset on the perimiter with that bit which I think was a mistake, or not needed. I air carved to check out my settings and found that it was starting off by plunging to the bottom of my 1.25 thick material and trying to cut the offset there......not good strategy because I probably would have had a failure of material or a bit. So I took the offset out and did not use any offset for the finish tooling . Maybe someone could enlighten me on that part of the process.