cancel
Showing results for 
Search instead for 
Did you mean: 

What is the best practice to avoid small cuts during REST_MILLING

Esteemed Contributor
Esteemed Contributor

In NX 8.5 we have always used the previous part stock value as the minimum removed material value to avoid small cuts with the REST_MILLING operation and 3D IPW.

Now with NX 10.0.3 MP14 we get a warning that there might be cut levels skipped due to the minimum removed material value being greater than the maximum cut depth. To our surprise the message was correct and there have been cut levels skipped, that would have resulted in the tool to cut the depth of three or more cut levels at once, which in turn would have resulted in the tool being turned into crap.

What is now the best practice to avoid small cuts when using the 3D IPW for REST_MILLING?

Thanks in advance for any pointers into the right direction.

Attached is a sample from NX 8.5 with programs with and without small cuts.

If you generate the tool path in NX 10 and above you should get the warning and the missing cut levels.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community
8 REPLIES

Re: What is the best practice to avoid small cuts during REST_MILLING

Valued Contributor
Valued Contributor

https://community.plm.automation.siemens.com/t5/Discussion-Forum-NX-Manufacturing/3D-REST-SKIPPED-CU...

 

I opened a topic about this issue before.My suggestion is that use your minumum material value as close as possible your depth of cut value.

-----------------------------------------
NX 11.0.2.7 MP1 / CanikSoft NC Post-Processing & G-Code Simulation
www.plast-met.com.tr
www.caniksoft.com

Re: What is the best practice to avoid small cuts during REST_MILLING

Esteemed Contributor
Esteemed Contributor

The problem is that this is a simplified body, the original is more complex due to the shape that is property of our customer.

As you can see from the image attached, we need to get rid of the cuts marked red.

Having to use a different setting depending on the cut depth was not satisfying in the past for more complex shapes.

 

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: What is the best practice to avoid small cuts during REST_MILLING

Valued Contributor
Valued Contributor

I understand you,I showed problem on an easy part before.İf you dont want to unnecessary passes on part you should use bigger min material removed value than previous operation depth of cut value.But problem is that İf you do that,some levels can be skipped according to your min material value.

 

So use safety value for min material value than edit unnecessary tool paths on part with tool path editSmiley Happy

-----------------------------------------
NX 11.0.2.7 MP1 / CanikSoft NC Post-Processing & G-Code Simulation
www.plast-met.com.tr
www.caniksoft.com

Re: What is the best practice to avoid small cuts during REST_MILLING

Valued Contributor
Valued Contributor

In situations simular like this one, I've set the stock value a little higher.
For example in this part set the stock to 1.6mm.

 

Also using IPW level based seems to help...


Regards,
Sven

NX11.0.1

Re: What is the best practice to avoid small cuts during REST_MILLING

Esteemed Contributor
Esteemed Contributor

SahinSanli wrote:

So use safety value for min material value than edit unnecessary tool paths on part with tool path editSmiley Happy


Tool path edit for a complex part is very cumbersome and time consuming. In addition you have to do it each time the design changes. This is really not a useful way for the future.

We really need something that can be used without user interaction in the future.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: What is the best practice to avoid small cuts during REST_MILLING

Esteemed Contributor
Esteemed Contributor

SvenV wrote:

In situations similar like this one, I've set the stock value a little higher.
For example in this part set the stock to 1.6mm.


Yes, currently this seems to be the only way to get rid of the possibility to crash the tool and/or the machine.

With the entire shape that was removed for this example, this needs a much bigger difference to get the expected result.

 

SvenV wrote:

Also using IPW level based seems to help...


This seems to be only reliable if the depth of cut is nearly the same for both operations, the previous and the rest milling one.

Would be nice to have one solution that is capable to succeed for 80-90% of the parts where such a strategy is needed. In NX 8.5 and lower this was the case, now we have to rethink many of the established work-flows.

A really fast preview of the tool path to expect would make it easier to check the result of using one or the other solution before one generates the final tool path. In many cases using a bigger depth of cut is not showing the short-comings of the chosen strategy.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: What is the best practice to avoid small cuts during REST_MILLING

Valued Contributor
Valued Contributor

I think that the origin for al these problems is the IPW resolution.
The IPW used for creating the rest milling operation is not acurate enough.

I tried changing the needle distance/count but that didn't seem to help, also don't fully understand what they do and if they are still used now that chordal tolerance is added.

 

Create the IPW using verify tool path with the choral tolerance set to 0,005mm

Then when u generate the rest milling operation the IPW form verify tool path is used and the results are much better without having to change stock or miniumum material removal values.

 

I also changed the in/outtol settings to 0,005mm.

 

image.png

 

Maybe with the new IPW update in NX11.0.2 this wil be easier...


Regards,
Sven

NX11.0.1

Re: What is the best practice to avoid small cuts during REST_MILLING

Esteemed Contributor
Esteemed Contributor

Thanks for taking the time to propose and test some solutions guys. Still not happy about the need to use workarounds, since I hear my users complaining.

Other parts of this project have about 200 operations, where the majority needs about 30 minutes for tool path generation and a few even 6 hours or more.

Going tighter with the in-/out-tolerance would increase the tool path generation times drastically, so not really an option.

Anything that needs special handling will not survive, since users tend to take the short-cut.

A more accurate and reliable IPW would be much appreciated.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Learn online





Solution Information