Router is not following g-code

[041414cbqi9449]

I'm using a shark pro hd 25x25x7 and have made a simple design in vcarve to practice. Every time I run the g-code the router barely moves in any direction. I'm not sure what to do exactly since I followed the tutorial to the letter. It could possibly be old software since no one has used the machine in years. I did however before designing my own ran a test file that came with the machine and it worked correctly but I've had no luck with my own designs.

If anyone has any tips or solutions i'll post the file below

Thanks, Trey

[041414cbqi9449]

whoops i uploaded the old file here's the edited one that i used to upload the toolpaths.

[Kayvon]

Can you upload the gcode file, too? I don't have VCarve installed on this computer, but I can take a look at the project file you've already uploaded when I get back.

Out of curiosity, isn't 041414cbqi9449 a difficult username to remember?

[nicksilva]

well the simulation and parameters look good so I'd want to take a look at the gCode as well.
BUT - lets get into tool selection. You've selected a vbit which regardless of the size the cutting is done with only the point. Sure the sides clear out area but the program only knows that the tiny tip has to cover every bit of the pocket area. I find that this is a problem with many beginners because no one explains the use of other tools. So I'm going to assume your .tap file is HUGE since it has to make literally thousands of movements to accomplish the goal - easily seen from the toolpath preview. Not to mention it will take a long time. NOW - compare that to the use of a 1/4 inch flat endmill which I tried. Here are the results. As you can see there are way fewer paths and it even did the insides of the B which the V bit did not. I think if you gave it enough time running, the vbit would have had larger swings as it hit the large clear areas. this is not user error by any stretch as it would eventually accomplish the task. You just need to experiment more with other endmills. I make LOTS of pockets and don't use Vbits for speed and clean flat areas. cheers!

[041414cbqi9449]

Thanks for the replies i didn't choose the username but i have it written down so I can't forget it.
I'll post the .tap files below

[041414cbqi9449]

pocket tap file

[James45]

make sure you are in the right units-inches/metric, correct post processor?

[Kayvon]

It looks like you're missing (or using the wrong) post-processor file.

The gcode files you've provided don't specify to the CNC what the units are, so the CNC doesn't know whether the gcode is giving it millimeters or inches. What's more, the first line of your gcode file tells the CNC machine to choose a particular tool, but Sharks don't have a tool changer, so that line is either ignored or the Shark just stops when it gets there.

A gcode file with the correct post-processor will have a nice header on the top and will set things up nicely for the CNC. I don't see any of that here--no default feed rate, no turning the spindle on or off (even router systems have these commands), no program end command.

Incidentally, when you're choosing the Shark post-processor file, you can choose either mm or inches and it will work fine. It's a common misconception on these forums that the units must match what you used to create the design. Not true at all--the software will convert the units for you, then the CNC machine will interpret those units and turn them into the same length. No matter which you choose, it'll come out correctly.

[nicksilva]

I agree you've used the wrong post processor but I think even if you did I suspect the same tiny movements would be generated.
while the file doesn't explicitly call out for metric or imperial movements my guess it has defaulted to inches. either way - first couse of action is to choose the correct PP.

[tonydude]

Use this post processor when saving toolpaths, since you are using mm

Tony