Selecting Cut Direction and Order

[LenMcC]

Two things I haven't been able to figure out are:

1) When I import my manually nested *dfx parts into Torchmate, how can I choose in which direction it cuts? It appears to default to CCW, but I'm cutting ODs, in which case CW is more appropriate to reduce bevel, right?

2) How do I select the cut order? I want it to cut the pieces "parallel"... first at the lower left, then the one to the right of it, then the one above it, then the one to the right of that, or in coordinates, (1,1)->(2,1)->(2,1)->(2,2), etc. I haven't figured out how TM determines what parts to cut when. I know the manual says something like "when optimize cut path is not selected, the parts are cut in order that they are recognized from the *dxf." Does this mean TM scans top to bottom? Because of our product and the material from which we make it, we need the parts to align exactly to our material. When TM cuts parts from the middle of the sheet first, or all along our material alignment fence, the rest of the sheet warps and botches the remaining parts.

[Mike@Torchmate]

Both of the settings you are referring to are done in the Torchmate CAD software. The cut Direction is set in the Toolpathing options when you are creating the tool path. There are two selections, Climbing and Conventional on the Basic Cut Tab. For plasma you would want Climbing because it keeps the right hand side of the torch moving away from you, on the keep piece of material, for your best dross and bevel.

Now the cut Order is set after toolpathing, either via the Start Sequence option, or you can enable the Show Toolpath Viewer under the View menu, on that screen there is a checkbox for Show Order. If you check this, each individual toolpath has a number assigned to it, which you can edit. 1 will cut first, then 2, then 3, etc...

[LenMcC]

good stuff. thanks for the quick reply!

[gfelippo]

My Logic tells me that applying the cut order through the CAD software means I have to save the drwing as a gCode. Is this true? If so, I still have not been able to use the gCodes saved from this Software (torchmate CAD). I export the drawing as .dxf and later import it to the Torchmate CNC soft. Should the cut order be maintained? Thanks!

Both of the settings you are referring to are done in the Torchmate CAD software. The cut Direction is set in the Toolpathing options when you are creating the tool path. There are two selections, Climbing and Conventional on the Basic Cut Tab. For plasma you would want Climbing because it keeps the right hand side of the torch moving away from you, on the keep piece of material, for your best dross and bevel.

Now the cut Order is set after toolpathing, either via the Start Sequence option, or you can enable the Show Toolpath Viewer under the View menu, on that screen there is a checkbox for Show Order. If you check this, each individual toolpath has a number assigned to it, which you can edit. 1 will cut first, then 2, then 3, etc...

[Mike@Torchmate]

My Logic tells me that applying the cut order through the CAD software means I have to save the drwing as a gCode. Is this true? If so, I still have not been able to use the gCodes saved from this Software (torchmate CAD). I export the drawing as .dxf and later import it to the Torchmate CNC soft. Should the cut order be maintained? Thanks!

No, the DXF file will save cut order, as well as XYZ location if necessary.

[gfelippo]

THANKS! Great info!

[LenMcC]

My Logic tells me that applying the cut order through the CAD software means I have to save the drwing as a gCode. Is this true? If so, I still have not been able to use the gCodes saved from this Software (torchmate CAD). I export the drawing as .dxf and later import it to the Torchmate CNC soft. Should the cut order be maintained? Thanks!

I initially found generating the g-code in TMcad to be confusing, but it's really pretty slick so long as you know the procedure. The nice things about generating the code in TMcad, particularly if you cut a lot of the same stock, is that you can make a toolpath template that already has the cut direction (you want CW or "climbing" for cutting male parts, CCW for holes), feedrate, lead-ins, etc. Then, when you open the file in TM, it's ready to cut.

Here's the procedure I wrote up for our parts (you may be able to delete some steps). Note that I offset the cut to compensate for the plasma kerf by directly editing the g-code in TM... Before the first G00 command, I insert "G41 D1". G41 offsets the tool path to the left of the cut, G42 to the right.

a. Go to File -> Import. Select your .dxf, and click on the blank stock to place the parts.
b. Move parts as a group to snap to left and bottom of stock.
c. Go to Machine -> Apply tool path -> Online. Select “default online template”, then “ok”.
d. Go to View -> Show toolphaths only and then View -> Show Toolpath Viewer and check the boxes for “Show Order” and “Show Direction”.
e. Select parts, go to Layout -> Ungroup.
f. Go to Layout -> Sequence -> Start sequence by list. Click on “Toolpaths Only”. Drag the lines of the parts list into the proper order following this convention: (not shown)
g. If its necessary to relocate the start point of the cut, go to Machine -> Edit Start Point and click on the toolpath where you want it to start.
h. Select parts, go to Machine -> Output. Click icon that looks like scissors on right side of tool bar.
i. Name & save .fgc file.

[LenMcC]

in TMcad, how do i make a lead-in? i can't get it to work by applying a tool path template, so i open "edit tool path" and apply it there, and again, it doesn't want to take.

[LenMcC]

nevermind, i got it. i was trying to apply the lead-in to "online" which i suppose doesn't allow the software to figure out which side of the line to insert the lead-in. selecting "male" did the trick.

[LenMcC]

I have my male toolpaths with the lead-ins. Now I want to change the starting point of each cut. But with the lead-ins added, I am only able select the lead-in or lead-out as the start point. Is there a way to move the whole lead-in/out?

edit: I figured out that if I go to "Machine" -> "Edit Tool Path", IF the blue nodes show up I can use the "Lead-In" button to move the lead-in/out. BUT, I can't figure our how to make the blue nodes show up sometimes... Sometimes "Edit Tool Path" kicks up the "Template" parameter window. Why do I get the nodes on some parts and the template parameters on others? All parts were imported in a single dxf, and had the tool paths applied all at once.

[jddurham]

Whenever you edit the tool path you will see in the edit toolbar a square w/ an arrow.
By selecting this tool this will let you move your lead-in and lead out point.
When you click on that box you will see a small red square on your page wherever you place that little red box and click your mouse that is where your leads will start and stop.
JDDurham

[jddurham]

After you have imported your DXF file if you don’t select all and make path (new Path)
Your path is broken (several little paths)
What you are seeing is all the different paths in you job
JDDurham