oscillating knife spins while cutting along vector resulting in broken blades

[jeffP4H2P]

does anyone else have this ongoing issue while cutting with the oscillating knife? it will randomly spin in circles while cutting along a line. curved or straight even some as simple as the file i've attached. it will spin on the left side near the only point on the curve. 

i'm using artcam 2015 insignia with an axyz router table. 

[Chetan.Bankar]

Hi @jeffP4H2P,

Welcome to the Autodesk Community and the ArtCAM Forum!

---

@jeffP4H2P wrote:

does anyone else have this ongoing issue while cutting with the oscillating knife? it will randomly spin in circles while cutting along a line. curved or straight even some as simple as the file i've attached. it will spin on the left side near the only point on the curve. 

i'm using artcam 2015 insignia with an axyz router table. 

---

What build of ArtCAM Insignia 2015 are you working in? To confirm this, select the Help > About ArtCAM Insignia menu option in your ArtCAM Insignia software. For example, ArtCAM Insignia 2015 R2.SP3 (64-bit build 860).

Please check whether there are any close or coincident points present in the vector at the position where the knife spins. If there are, please try editing and removing one of the coincident/close points from the selected vector, re-calculating your toolpath, and then post processing the toolpath again to see if it resolves your reported issue.

If still you encounter the same issue, then please provide us with your ArtCAM Model file (*.art) and confirm which post processor you are selecting when saving your toolpaths so that we can investigate further.

Thanks and regards, 

[jeffP4H2P]

I'm using artcam insignia 2015 64bit build 244

I tried removing the single point on the left side and it worked. the knife didn't spin.

How can I catch this issue before it gets to cutting and ruining both my cut and breaking my blade? I can't see anything wrong with the file before I cut. 

I've attached the artcam file

thanks for your help.

[dillon.moulder]

Hi @jeffP4H2P,

---

@jeffP4H2P wrote:

I'm using artcam insignia 2015 64bit build 244

---

You aren't working in the latest version and build of ArtCAM Insignia available to you.

Please use the following steps to download and install ArtCAM Insignia 2015 R2.SP3 (64-bit build 860) on your computer:

1. Shut down all sessions of ArtCAM Insignia currently running on your computer.
2. Visit the Autodesk Customer Downloads Centre.
3. Enter your dongle number and registered email address, then click Submit. A Customer Verification email is sent to your registered email address.
4. Click the link included in the Customer Verification email to access the Autodesk Customer Downloads Centre.
5. Click the ArtCAM link in the site's left column to display the customer downloads for ArtCAM.
6. Click the ArtCAM 2015 R2 – Full Install link to download the ArtCAM_2015.813.Full.zip file.
7. Click the ArtCAM link in the site's left column to display the customer downloads for ArtCAM.
8. Click the ArtCAM 2015 R2 Service Pack 3 – Minimal Install link to download the ArtCAM_2015.860.Minimal.exe file.
9. Extract the downloaded ArtCAM_2015.813.Full.zip file on your computer using 7-Zip or WinRAR.
10. In the extracted ArtCAM_2015.813.Full folder, right-click the Setup.exe file and select the Run as administrator context menu option to install ArtCAM Insignia 2015 R2 (64-bit build 813). Allow the installation process to complete.
11. Right-click the ArtCAM_2015.860.Minimal.exe file, then select the Run as administrator context menu option to update to ArtCAM Insignia 2015 R2.SP3 (64-bit build 860).

Thanks in advance for your time and cooperation.

Kind regards,

[jeffP4H2P]

Ok I'm upto date now. Still same issue however now I've lost my toolpath menu too and can't find anywhere to turn it back on. 

I did notice that if I use "outside" instead of "cut along vector" it cuts in the opposite direction and doesn't spin. I've only tested on this file though so I don't know if it's unique to this vector or not. 

[Chetan.Bankar]

Hi @jeffP4H2P,

---

@jeffP4H2P wrote:

Ok I'm upto date now. Still same issue however now I've lost my toolpath menu too and can't find anywhere to turn it back on. 

I did notice that if I use "outside" instead of "cut along vector" it cuts in the opposite direction and doesn't spin. I've only tested on this file though so I don't know if it's unique to this vector or not.

---

I'm glad to hear that you're now working in ArtCAM Insignia 2015 R2.SP3 (64-bit build 860). 

Please confirm whether your supplied ArtCAM Model file (knife samlpe.art) is the original model, or a modified one. In addition, please confirm which of the nodes in your vector have been deleted, and the name of the post processor you're selecting when saving your toolpaths.

The reason I ask this is because I have simulated the toolpath in your supplied ArtCAM Model file (knife samlpe.art) and it doesn't spin during the simulation. I've used a bigger tool diameter for the toolpath simulation; since the Along profile type has been used, this shouldn't effect the final NC output.

I'm not clear about the issue you've encountered with the Toolpath menu. Are you perhaps unable to find the Project panel in the ArtCAM software interface? If so, please try the following steps:

1. Select Window > Toolbar and Docking Windows and ensure that the Project menu option is selected.
2. In Windows, select Start > All Programs > ArtCAM 2015 R2 then select the Reset ArtCAM 2015 R2 Workspace option.

Afterwards, please restart ArtCAM and confirm whether the missing menu is displayed. If this is not the issue you're trying to describe, then please provide further information.

Thanks and regards,

[dillon.moulder]

Hi @jeffP4H2P,

---

@jeffP4H2P wrote:

I've lost my toolpath menu too and can't find anywhere to turn it back on. 

---

The Toolpaths panel was removed in ArtCAM 2015 R2; all of its functionality is available from the Project panel. Please select the Help > What's New menu option in ArtCAM Insignia 2015 R2.SP3 (64-bit build 860) and read the Miscellaneous changes section of the documentation.

If you have any further questions, please do not hesitate to ask. Thanks in advance for your time and cooperation.

Kind regards,

[jeffP4H2P]

This was the original model file. The node I was removing is the single node on the right side. 

I've also noticed that it doesn't spin during the simulation. This is was so frustrating about the issue. At $50-$75 dollars a blade it can get to be a very expensive problem while cutting inexpensive materials. 

What is the post processor? 

[dillon.moulder]

Hi @jeffP4H2P,

---

@jeffP4H2P wrote:

This was the original model file. The node I was removing is the single node on the right side.

---

There are two nodes on the right-hand side of the vector artwork within your supplied knife samlpe.art file, as shown below:

 

Previously, you mentioned removing a node from the left-hand side:

---

@jeffP4H2P wrote:

it will spin on the left side near the only point on the curve. 

---

---

jeffP4H2P wrote:

I tried removing the single point on the left side and it worked. the knife didn't spin.

---

Please confirm which of the nodes you are removing using a screenshot.

---

jeffP4H2P wrote: 

What is the post processor? 

---

The post processor is the option you select from the Save Toolpaths dialog's Machine file format list when saving your toolpaths from ArtCAM Insignia 2015 R2.SP3 (64-bit build 860). For example, Axyz_MultiTool_Arc_MM (*.nc).

Thanks again for your time and cooperation.

Kind regards,

[jeffP4H2P]

The post processor is AXYZ_A2MC_INCH(*nc)

it's the bottom node in the diagram you sent. 

thanks 

[Chetan.Bankar · Accepted solution]

Hi @jeffP4H2P,

---

@jeffP4H2P wrote:

The post processor is AXYZ_A2MC_INCH(*nc)

it's the bottom node in the diagram you sent.

---

Thanks for supplying the required information. With knife cutting, ArtCAM outputs only the co-ordinate values (using the AXYZ_A2MC_INCH post processor) for the given vector; the knife tangency must be maintained by the controller.

I initially assumed that the reason for the knife failing to retain tangency within that short distance was due to two co-incident points (causing the loop in the close vector) or two very close points (the knife has its own width), but with the information you've provided that does not seem to be the case.

I suggest that you to try the following steps and check whether it makes any difference by dry-running (without any material loaded) the output:

• Arc fit the vectors to be machined by the knife and then create the toolpath.
• I assume that you are using an A2MC controller on your Axyz machine, so you have selected the correct post processor. The post you are using correctly outputs co-ordinates to the 4^th decimal, but it also outputs in absolute arc co-ordinates.

If your machine supports incremental arc output, then I suggest that you select the Axyz_MultiTool_Arc_INCH (*.nc) option when saving your toolpaths; this outputs incremental arc co-ordinates.

• Check whether the tool's initial angle is specified correctly on your controller.

In my experience, to avoid such a problem while knife cutting, it is advisable to keep the vector artwork as simple as possible. I also suggest that you keep the vector's curved spans as arcs or beziers to confirm whether these type of vectors enable your controller to keep the knife tangent throughout without spinning.

Thanks and regards,

[jeffP4H2P]

The two solutions I've found to work in this case was to either cut using "outside" instead of "along vector" and/or arc fit the vectors. 

thank you both for your help!

[jeffP4H2P]

I just tried this with another file I had and the only solution that worked on all shapes was fit arcs to vector.

If i cut outside & climb I get the issue and if i change it to conventional it's fixed.