Manually cutting a shape in middle of board??

[Ian Richardson]

Hi, new here. Learning every day. I have a question. Here's the scenario: I have a 36"sq piece of 3/4" mdf. I would like to cut a 6"x 6" piece out of it. If I was to input this info manually then nest it. It would nest the piece on the corner. What if I wanted to have it nested in a certain area of the board? Can I choose an x and y point from where it would start to cut? Lets say 8"(x) and 10"(y).
Thanks for the help.
Ian

[Scott Marshburn]

Could you clarify what you are wanting to do. Are you wanting to cut a 6"x6" pocket out of a part that is 36" square or are you just needing to cut a 6"x6" part from a 36" square sheet?
The way that I would do this If I was wanting a 6"x6" part from a 36 inch square sheet and needed to cut it from a particular location . would to be draw the geometry in a cad program putting the 36x36 geometry on a Outline layer and then the 6x6 part on a chain compout layer at the location that I wanted to cut it at. Then at the controller I would select scrap part recovery nest to edge and no outline cuts.

[Daniel Odom]

You could also nest it to the corner and use a fixture offset to move it to the center or use a really big collar value. You can set up a material type to do this automatically. If you have to nest several items in specific places then Scott's suggested method is the better way.

[Ian Richardson]

Sorry for the confusion. Should have drawn this first. As you can see a 36" x 36" panel with a 6"x6" cut out in the middle. I have Solidworks, I thought there might be a simpler way to "fool" the machine to tell it where to start.
Thanks
Ian

[Ian Richardson]

You could also nest it to the corner and use a fixture offset to move it to the center or use a really big collar value. You can set up a material type to do this automatically. If you have to nest several items in specific places then Scott's suggested method is the better way.

Thanks Daniel, could you clarify a fixture offset and collar value? Sorry for the newbie questions

Cheers

[Daniel Odom]

This may be difficult to explain, but here goes: At the machine you can program 0,0 of programs to be wherever you want, your default position is where the pop up pins are, you can move it away by programing a new 0,0 for the machine to reference during the program. You can nest your part to the lower left of your sheet and then change the default 0,0 (usually G901 or G52L1)to use a different part location reference to run from (G52L#whatever) during the program, thus moving you part to another part of your sheet depending on how you offset in x and y. This works because your sheet will still be at g901/g52l1, the machine only thinks it's in a different spot. You'll need to look up the value of your g901 or g52l1 and subtract from that number to move away from it. This will only work in you nest to edge in the lower left of sheet w/out collar and use a fixture offset.

For multiple parts just add a collar in control nesting settings; this is the distance from the edge of the sheet the parts can't nest to, it works in an equal distance from all sides of the sheet. So you put 10" in and parts will nest 10 inches away from each edge. This way requires a little trial and error to get it the way you want.

[Scott Marshburn]

If you use a fixture offset then it will move the sheet witch is to my understanding 36"x36" by the offset value .this will not move the 6x6 part just the sheet. The collar could be increased for example a 8 inch collar but this collar would be applied on x and y . so if you wanted the 6x6 part cut 8" on the x and 10" on the y this method would not worke.The drawing that you posted shows a large rectangle black lines (is this your sheet?) a smaller square "red lines" ( is this part going to be cut from the sheet?) and a smaller square "blue lines"( Is this a pocket/square hole or the actual part you are wanting to cut?)

[Daniel Odom]

Maybe I'm not explaining clearly, but it does work, I do it all the time. The sheet moves and the part is in lower left, in reality you place the sheet in the non moved position, so when cut the part is cut in the offset position. It sounds more complicated than it actually is. I'd post a video if I had time but I'm usually too busy. Not sure what you mean about the collar.

From looking at ops drawing it seems not to be a nesting of a part but the part itself. If this is the case you simply draw the part and use dxf nesting and choose no outline.

[Ian Richardson]

Actually Scott the large black rectangle represents the table. The red is the 36" sq sheet.
Thanks for everyones input. Much appreciated. Will play with ideas on Monday.

Ian

[Scott Marshburn]

Daniel I understand the method that you described and have used this in the past. But it requires too much math and setup time. (That is for me any how). Also If the 36x36 changes lets say you set up for a 36x36 and you cut 6 pieces. Then next week you need to cut 6 more and this time the 36x36 part is 36 1/2 x36 then you have to create a new offset or change the one used before. It is just easier for me to use dxf layers for this type of cut.Ian if the 6x6 square is a pocket the 36x36 part could be drawn in eCabinets (If you have it) using a cabinet back and then put a 6x6 pocket and constrain it to the center of the back this way if the 36x36 part needs to be resized the pocket would remain in the center. Unless I am wrong you could then nest the 36x36 part using scrap part recovery and no outline cuts.

[Daniel Odom]

Oh, I agree, I only do it that way for specific reasons, usually for locating a part using wood dowels instead of the metal fence for flip op or other secondary operations, jigs etc. I actually use G902 for this, I have a shortcut to the M999 macro and just use a minus sign after the x and y locations and move however much is needed for that setup, save and re-calibrate. This only works for nesting one part or temporarily offseting a sheet, say there's a bad spot on the edge of one sheet in the bundle after you've already nested, for example. I guess I've been doing it for so long it doesn't seem that complicated to me, but I can see how it would be confusing in some ways.

What I meant about the collar was that you can nest multiple parts to a general middle area of the sheet (not exact in any way shape or form), if you needed to for some reason. I think I just misunderstood what op was getting at, thinking he wanted to nest one part in a specific location, not make a part with a cut-out in a specific location, that changes everything. In that case the part and the sheet are the same thing, so nest to edge with no outline cuts and your done.

Sometimes when I nest parts using of other cam software I do the same thing; nest everything in that cam program but use chain compout layers for the parts instead of outline layer and use the sheet as the outline layer, then nest in control nesting, no outline.

[Kerry Fullington]

Ian,

To accomplish these type tasks I created a flat panel stock in eCabinets that is simply the back of a cabinet with all other parts removed. (make sure you make the back flush before removing the other parts) This can now be re sized to your panel size such as 36 X 36 in your case.
I took the panel into the part editor and cut a random square cutout using geometry. Size and position are not important at this point.
Exit the part editor and take the panel into the Constraint Manager. Here you can apply vertical and horizontal constraints to your cutout and from the part corner to the cutout. You can resize the cutout and change the position of this cutout by editing these constraints.
Once your cutout is properly sized and positioned just create a twd and nest it. Be sure to use Nest to edge of part so that your 36 X 36 panel does not get trimmed.

iantest.jpg (4.56 KiB) Viewed 13374 times

[Dennis Englert]

Assuming that you are only cutting the 6" square from the 36" square, I would just write a program. There are a number of ways to do this and Kerry offered a very good method. You do not need to be fluent in G-Code and if need be, you can edit the size and location of the square in eCabinets, then recreate the CNC file.

But if you were to write it, it would look something like this.

(Program Name: )
G90
SET ZSHIFT = .75 (MATERIAL THICKNESS)
[ADJFIXOFF, 1, -36]
[ADJFIXOFF, 2, -36]
G52L1 (FIXTURE OFFSET FOR POPUP PINS)
T1 M03 (REPLACE THE TOOL NUMBER WITH YOUR TOOL NUMBER)
S18000

G00 X18 Y15
Z.25
M31

(CLIMB CUT)
(MUST START FROM EDGE OF SQUARE, NOT INSIDE CORNER FOR TOOL COMP)
G91
G41
G01 Z-1 F100
X3 F200
Y6
X-6
Y-6
X3
G00 Z1
G40

M05
G990
G90
G00 Z0
X0 Y0
M02

If you are familiar/comfortable with G-Code, then it is often quicker to write the code, than it is to go back to your desk, design it in software, generate the CNC file and run back to the machine to load and run the file.


Dennis
Dennis

[Kerry Fullington]

Dennnis,

I have these Panels, (with and without grain in various thickness materials) saved on the control to use with Quick Cut to cut the odd shelf etc. out of scrap. Because of this I can open the panel in ecabinets on the control and do all editing and write the twd from there. It can also be saved as a Quick Cut part for future use.

[Daniel Odom]

The advantage to writing this in g-code would be that you would have more options for making the program with parametric constraints than with the constraint manager in Ecabinet systems; as well as looping, prompts etc. I tend to draw faster than I can write g-code (without making a few bonehead mistakes anyhow) so I only use parametric g-code programming when I'm doing a lot of parts with slight variation; would not recommend for a one-off. That is unless your part is as simple as this example, mine seldom are though.