Problem with Cut 3D Software

[bretmi]

Wanted to see if anybody knew or has ran into having a problem using a file on sample disk-> creating a tool path and putting it in the CNC Shark post processor in inches and then go to cut in and have the machine move all the way to the corner of the X Y axis and stop working. Has anybody had this problem? If so, how do I go about fixing it?

[fred1030]

Even though I am brand new with the Shark and Cut 3 D, I seem to be having the same problem. I even bought a Vector Art 3D file, loaded it, ran and saved the toolpath files but when I loaded the .tap file in the post processor all it will do is move the router maybe 1/2 inch after running the complete file. I bet yours is doing the same thing. If you look closely at your bit, I bet it is moving but just barely.
WHAT ARE WE DOING WRONG? Can someone give us some advice or help.

[jeb2cav]

Hi - can either of you please post your Cut3D project file so we can look at it?

[fred1030]

I tried to send files twice but guess they did not come through.

[jeb2cav]

Fred's project file was too large to attach and I should've thought of that. We were able to arrange a file exchange outside of the forum...

Looking through the Cut3D file (its extension is .v3d), I noticed early on that the x and y origin were set to -76 and -73. I'm not sure how they got that way - it could be that the model itself had an odd origin, and when it was first imported into the Cut3D project, these values got set accordingly. In either case, in the Cut3D panel, the x, y and z values are similar in nature to how you set them in VCarve or Aspire - they are where you are going to set your tool to define 0,0,0. This pic shows the original values (the x negative sign is hard to see for some reason, but it was negative).

X and Y Origin Position Settings in Original Cut3D Project

I set these to 0, 0. The z value was set to top of material in this project. I didn't notice any other settings that I would change. I did recalculate the toolpaths though as I changed the x,y origin.

When I generated the tap files at the end, I compared them with the ones Fred had provided. You can see that the tool is moving to locations that make more sense (the model is ~7.2" tall and ~7" wide). This pic shows the 2 tap files side by side - at the beginning of their respective cuts.

Roughing 3D Pass Tap Files - Original and After Origin Change

I think you were getting such a small movement as the tap file was too confusing or out of bounds. I didn't run the tap Fred sent, but I'm curious if the gantry ran to the extents until it got to -76. I think a tap file is too hard to really go through line by line. However, looking at them sometimes for a few things can be useful in trying to figure out what is going on - and then that might give you a clue as to where to look in your project and make the adjustment. In this case, seeing that the machine is trying to go to -69, -73, 0.2 is a sign that something's not right, probably with the origin. Even on the ProPlus, you're working with a 24" x 44" table (or thereabouts).

I don't have a lot of experience using Cut3D or VectorArt 3D Machinist, as I went fairly quickly to Aspire. Aspire can do all of this stuff without use of either of these 2 programs (and it can also use their project files as VCarve does). But, I do like to bring these into VCarve as I typically am adding text or other composition components to my project. So, I import the Cut3D *.v3d file into VCarve. In this case, when I imported the original v3d file into a VCarve project, and looked at the 3D view with the toolpaths turned on, I see that the model is well off my workpiece (and machine in this case).

Original Cut3D Project File in VCarve Pro

Ok - 3 attachment limit, continued in next post...

[jeb2cav]

Continuing from previous post -

When I import the revised Cut3D project v3d file (0,0,0), and view it in the 3D view with the toolpaths enabled, I see that it is where I expect it to be.

Cut3D File in VCarve Pro after xyz Zero Adjustment

A few more notes on the rest of the workflow in this case - ie I imported my Cut3D project into VCarve, and then I moved it to the desired location. So, in the next picture, you see where I moved it in this project (compared to pic above). You also note that at this point the tool thinks the origin is now somewhere in the middle of my project (circled).

Cut3D File in VCarve after Moving It - Note Toolpath Origin

Note: I've later come to the knowledge that the next step is not required. I've left it in for truth in advertising. VCarve Pro does the 'right thing' with the toolpath based on where ever you end up positioning the 3D component in your VCP project design. You still need to use the same origin in your Cut3D project as you are planning to use in the VCarvePro project. So, you don't need to: After you import a Cut3D or VectorArt 3D Machinist file into VCarve or Aspire, you need to open up each of the associated toolpaths and hit the apply button. You won't be regenerating the toolpaths over the model, but you will be updating the material origin now in play - and you must do this otherwise that model is going to end up in the "wrong place".

Apply New Origin to Cut3D Project in VCarve

3 attachment limit, one more post...

[jeb2cav]

3rd and last post in response -

So, after hitting apply, you can see that the toolpath is now starting from this project's material origin (lower left corner in this case)(and the screen grab is a little misleading as it looks like it is not ending on the corner - remember that the tool is starting 0.2 above the material when the router turns on, and that is causing this pic to appear "off").

After Applying New Origin to Cut3D project in VCarve

Another post on this kind of workflow is http://www.cncsharktalk.com/viewtopic.php?f=10&t=387. It doesn't address the problem you experienced, but may provide some additional insights into the 2.5D modeling aspects of VCarve Pro and how Cut3D or VectorArt 3D Machinist fit into that.

Hope this cures it - I didn't test drive the new tap file, but think this will resolve the problem.

[fred1030]

Thanks a lot.
Between what advice you gave me and reloading the second time the proper postP file into the program and recalculating the cut runs, I think I am about to begin again. I experimented on a small project and it worked fine.
Now I think I am about to cut my indian friend out in a 1 inch piece. I will take almost 6 hours cutting time. Wish me luck
Fred
and again
Thanks