Using sink dxf in CNC

[RANDYMURPHY]

Hi, brand new CNC operator here. We would like to use sink dxf files downloaded from manufacturers' websites to create a digital path for the CNC machine to follow (We have a Park Industries Destiny machine).

As you know, dxf files need to be edited in CAD to remove all of the extra text. I'm having trouble creating the lead-in path for the mill bit to follow to being that inside cut. Do any of you have experience with this? Or rather, do any of you use .dxf sink drop in files for this purpose?

We'd like to take a dxf file of a sink cutout from a manufacturers' website and transfer it to our CNC machine from Park Industries, which the CNC will use to cut out the sink hole. The dxf files do not include lead-ins, though. I'm trying to use the LT-55 software to draw arcs in the center of the sink to create the path the milling bit will take. However, the CNC machine is not recognizing that the new arc (lead-in) and the oval sink are combined. It only wants to cut the arc lead-in, and then stop. I have looked at the file in CAD to make sure that the template is all at the 0 level.

Like I said, I'm new at digital templates, so I hope I've explained myself clearly enough. I've attached the .dxf file that I've been talking about.

Thanks

[Mark Meriaux]

I'm not a CNC programmer, but I've seen thousands of DXFs and sink files.

The LT55 software is a very simple and easy-to-use CAD program for drawing simple shapes and editing files created with their laser. I'd venture to guess that your CAM program would be a better option for assigning tool paths (not the LT-55XL software). Over time, you will build up a library of just the sink outlines that you use. Most of all tool pathing that I've seen is done in the CAM program, after a plain line DXF is imported. The CAM software (AlphaCAM, etc) is where designate which side of the line gets cut (inside or outside), and it also determines offsets for the overmaterial that is left for the subsequent tools to remove.

We've got and awesome group of SFA members that will share their working DXFs for every member to download in the DXF Forum. A great thread to start with is Joe Durfee's entire DXF library which is downloadable within this thread:
http://forum.stonefabricatorsalliance.c ... =38&t=4426

Hopefully some others will chime in and give you better help with your file.

Happy programming!

[countertopperscnc]

I had that problem a few times and modify the .dxf files in autocad instead of on the xl. Normally when I have the problem the sink is a closed loop. you need to "explode" (a command in autocad)the sink path you want. then using autocad draw an arc from the point you want on the sink to a place usually 3 inches or more inside the sink path. If your cutter will follow the same line twice be sure to make a copy of that line on itself. Message me with your number if you want me to call and explain further.

[badboat]

If using Alphacam you can modify your toolpaths after you assign them under the Machine tab, then go to tool lead in/out. Select arc in both windows and then move the arc to where you want it to lead in and out.

[Nick]

Not sure I follow what you want, but if it is lead ins regarding tool path, that happens when you apply your tools.

[VThartzog]

Usually your cnc software will use pre programmed leadin leadout values that do not need to be programmed, but are preset in your tool settings. I think Dan Dauchess runs a destiny and might have a little more insight, but you shouldn't have to programs arcs to serve as lead ins/outs

[Ken Lago]

Yeah Dan D's Destiny is a very basic cnc and have needs that newer models don't have.

[countertopperscnc]

modified your sink a little.

[MikeM]

I tried importing your file to our OdysseyII. The machine indicated a break in the tool path (I don't remember exact wording of the message). I used my CAD program to find the problem. Your lead-in arc was not quite attached to the rest of your tool path. Also when you have a line between your lead-in and lead-out, that line is used once at the beginning of the cut, but cannot be used again at the end of the cut to get to your lead-out arc. So you have to put a second line over that line connecting your lead-in and lead-out. Hope that's clear.

I usually try to connect my lead-in and lead-out to the same point if possible. If not possible, I double up the in-between segment which is usually an arc in the lower left corner of the cut-out.

The CAD program I use is a 10 year-old version of TurboCad which I got years ago on Ebay. I use it for adding lead-ins,outs, and creating tool paths for islands and vanities (when they have curves). For this I use lines, arcs and fillets, that's about all I need. Think I paid about $40.

One other note about your dxf file. It is all line segments. I never have used one like this. A template like that I would usually do using 8 arcs.

Hope you find this of some use.

[H. Adkins]

If you use autocad you can join all the segments by using the "pe" or "pedit"command.
In the command line type

Command: pe
PEDIT Select polyline or [Multiple]: m
Select objects: Specify opposite corner: 50 found
Select objects:
Convert Lines and Arcs to polylines [Yes/No]? <Y> y
Enter an option [Close/Open/Join/Width/Fit/Spline/Decurve/Ltype gen/Undo]: j
Join Type = Extend
Enter fuzz distance or [Jointype] <0>:
47 segments added to 2 polylines

Our Park Titan would have trouble with all those segments. I would draw an ellipse.

Most CAM software should draw the leads for you. When we first starting using a cnc, we used Synergy (sp?) to do our programming and had to draw all the leads. It was a pain in the A**! Now we use AlphaCAM & it's a piece of cake.

[BobbyC]

I program our park destiny. If you still need some help call me in the morning.

434-531-1711
Wes

[Dan Dauchess]

Wes/robert can help you with stone am. I've got an odyssey and can help with the cad issues. The odyssey/ destiny are dumb and you need to add the lead in/out to the tool paths in cad. The suggestions above are good starts.

Call me at 757 570-4632