2d view question

[highpockets]

Steven, give this one a try....

2D View Question - Moulding.crv3d

(582.5 KiB) Downloaded 77 times

I circled the drive rail in RED it's only .005" high.

[dealguy11]

It's pretty simple, though you'll have an issue at the vertical areas because when it gets to these places it will immediately plunge the bit into the material, possibly breaking the bit. That said:

1. Set up your material with the width along x equal to or greater than the length of your part. Set up the height along y to some small number, perhaps 1 inch (doesn't really matter). Set the xy datum position so that x goes through the center of the material and y0 is at the head end of the material. There is no need to set this up as a rotary project, just keep it flat.

2. Use your profile vector to create a 2-rail sweep. The rails of the sweep will be at either end of the part and just need to be long enough to generate the shape. The profile vector is the sweep vector. Center this part vertically so that the x axis goes down its center.

3. Draw a straight line from x0y0 to the end of the part on the x axis.

4. With the component from step 2 visible and the vector from step 3, create a profile toolpath that cuts 0 depth, with "project toolpath onto 3d model" checked on. If it were me I'd set the feedrate pretty slow and the spindle speed very high.

That's it.

[TReischl]

Essentially, if I am reading this all correctly, you are wanting to program a lathe.

Lathes only use X and Z axis (we all knew that). Well, back about a half a century ago I programmed a lathe that was Y and Z. Actually, that may still be the standard. I have not programmed one since about 1975.

What you could do to get that profiling pass is go ahead and draw it up as if you were doing a normal XY profile cut.

Post the file.

Load the file in a text editor, notepad works fine, All of your X's need to be changed to Z's. Mass edit. About 4 decades ago I programmed an NC lathe. Best thing to do is put your 0,0 on the centerline of the part. Then draw the part so that all of it is to the right of your 0,0. That way if you see any negative Z moves you know you are going to hit the chuck. You can also set the 0,0 at the top of the round blank. Not advisable.

[adze_cnc]

Load the file in a text editor, notepad works fine, All of your X's need to be changed to Z's. Mass edit.

I suspect the appropriate post-processor could be modified to do that for you.

[ger21]

Hi yes I need to explain it a bit better sorry : imaging you have a 3d carving of a face on a board, I just want to carve one of the vectors along the Y or X + the 3d heights on the Z . In other words I want to draw a single vector of various heights and curves etc (the Z), and project it along the X or Y. A single vector of the 3d model.

Aspire does not allow "3D" vectors. Only flat 2D vectors.

The easiest way to do it would be to write a custom post that swapped Y (or X) for Z, and draw it in the XY plane. To be accurate, you'll need to allow for the radius of the tool when cutting from above, as it will gouge if you don't.

[highpockets]

It's pretty simple, though you'll have an issue at the vertical areas because when it gets to these places it will immediately plunge the bit into the material, possibly breaking the bit.

Good point. To use the Moulding toolpath just use the "Use Larger Area Clearance Tool" specify the same size tool and when saving Toolpath just save them together. The clearance will run first then the finish.

[Rcnewcomb]

An alternate approach is to do the cutting from the side rather than the top. ->Video example

[dealguy11]

This has been an interesting discussion. As with everything in Aspire, there are generally at least 3 ways to accomplish a task. Choose the method you like!

I do think the approach using a 2-rail sweep is how I would go, for the following reasons:

1. I don't like to mess around with working post-processors. Not that it can't be done, and I know of cases where flipping axes for rotary work makes a lot of sense, but I don't think it's needed here.
2. You can get crisper details cutting down from the top rather than coming in from the side, because you can generally use smaller bits (as long as you don't bury them). If you do flat portions of the profile with an end mill rather than a ball-nose cutter, then you can get nice sharp inside corners in those areas.
3. It doesn't require Y movement, which was one of the OP's goals.

But hey, whatever works.

Some other things to consider. I'm 100% in agreement with TReischl that you should set z0 to the center of the turning blank. You need to turn the blank round before you begin. I've always found a 1.25" bottom cutting bit like the Magnate 2704 is a good choice for that operation. If you use my method, make sure the profile path is on the vector, not inside or outside. If you have any option for y movement, consider offsetting the vector to the side for the turning round operation so that the center of the bit is not directly on top of the part...if the part is turning into the bit, you will get a smoother cut but this only works for a flat bit. Do hog out as much material as possible before you do the final profile. This operation is actually kind of hard on a rotating bit because the feed rates are inflated by the material moving past the bit...that's why the spindle speed needs to be high.

[Fivetide]

Steven, give this one a try....

2D View Question - Moulding.crv3d

I circled the drive rail in RED it's only .005" high.

Image 342.png

Thanks John Ill give this a try..

This has become more complicated than I thought lol

The swapping of the axis code may be a start Ill just swap the wiring around that's pretty simple.
I was thinking of a pocket clearance tool path first
Or the alternative is to do a rotary wrap and try that and take out the rotating part of the code .. that should leave me with the Z + Y part of the code.
I can dry run all your suggestions on the desk I haven't attached it yet.
Thanks to all for the suggestions, much appreciated.
If I work out a good simple solution I'll post it in this thread to help others.
BTW this was what I meant when I was talking about a 3d model something along those lines, if the 3d model was 12mm wide along the X and I used a 12mm end bit I assumed it would generate one X path How to Mill a curved surface and engrave text onto it https://www.youtube.com/watch?v=rX6GO4Z3LWg&t=5s

[Fivetide]

This has been an interesting discussion. As with everything in Aspire, there are generally at least 3 ways to accomplish a task. Choose the method you like!

I do think the approach using a 2-rail sweep is how I would go, for the following reasons:

1. I don't like to mess around with working post-processors. Not that it can't be done, and I know of cases where flipping axes for rotary work makes a lot of sense, but I don't think it's needed here.
2. You can get crisper details cutting down from the top rather than coming in from the side, because you can generally use smaller bits (as long as you don't bury them). If you do flat portions of the profile with an end mill rather than a ball-nose cutter, then you can get nice sharp inside corners in those areas.
3. It doesn't require Y movement, which was one of the OP's goals.

But hey, whatever works.

Some other things to consider.
I'm 100% in agreement with TReischl that you should set z0 to the center of the turning blank. Yes this does look like the best way to set the z0
You need to turn the blank round before you begin. I've always found a 1.25" bottom cutting bit like the Magnate 2704 is a good choice for that operation. If you use my method, make sure the profile path is on the vector, not inside or outside.
If you have any option for y movement, consider offsetting the vector to the side for the turning round operation so that the center of the bit is not directly on top of the part...if the part is turning into the bit, you will get a smoother cut but this only works for a flat bit. Good Point thanks
Do hog out as much material as possible before you do the final profile. I need to experiment with clearance tool paths or pocketing before I do some actual material cutting
This operation is actually kind of hard on a rotating bit because the feed rates are inflated by the material moving past the bit...that's why the spindle speed needs to be high. The lathe only has 3 manual belt speeds unfortunately so the feed rates will have to be worked out as buy chewing through a few experimental blanks lol and thanks yes another good point.