Cancel
Showing results for 
Search instead for 
Did you mean: 

Cutcom issues NX9 milling

Creator
Creator

Hi all,

 

Only my second post so bear with me please.

 

I have been using NX9 for a few months now in my new role. I have been on the basic CAD and CAM courses so can get by and have been programming on Mastercam for over 10 years so would like to think I am half decent at CAM.

 

My problem is with tool compensation. We manufacture complex shaped slots which vary from 0.5mm wide to 2mm+. These often follow a spline curve which can vary in X, Y and Z simultaneously. They also are often radiused in the bottom and the width also narrows towards the front/back of the slot (to take a swaged hypodermic tube).

 

In the past my company have got by with using a datum shift on the machine to obtain the correct slot width, these are often tied down to around 10 microns.

 

I am currently trialing using SOLID PROFILE 3D, which gives me the option to pick the side walls and follow the bottom of the wall. So far, so good, however when I choose cutter compensation, no matter how small i make the moves or angle, due to the fact I need to start or stop mid slot before I hit the narrower sections, it throws up an alarm:

"The requested minimum move or angle for cutter compensation could not be made safely, cutcom statements were output with available engage and retract moves".

 

I guess my question really is am I using the correct operation, is there a better one or is there something I can adjust or ensure is set to help me cut these slots without having to have seperate programs and datum shifts on the machine.

 

I have attached some screen dumps to try and show an example component. The slots on this part are 0.71mm wide for the back (10mm long), 0.8mm wide for the central section and 0.654mm wide for the front (10mm long). They travel in X, Y and Z and have full radius at bottom (also different depths dependant on width).

 

Thanks in advance.

 

Matt

9 REPLIES

Re: Cutcom issues NX9 milling

Legend
Legend

Try turning off collision checking in the non-cutting moves. Just be sure to carefully make sure there are no collisions in the path. See if this helps. 

 

 

 

Edit:

 

I wanted to re emphasize that if collision checking is off, that you very carefully verify the path. I even switch the graphics to wireframe or set it temporarily transparent to make sure the path does not dive into the part. When the model is viewed as solid it is very easy to overlook a gouge. 

 

Also, at the end of verifying, I use ctrl-W, and then toggle the solids on and off. Gouges are easier to detect this way. 

 

Glenn Balon
Production: NX 12.0.1.7 MP1 Primarily CAM

Re: Cutcom issues NX9 milling

Genius
Genius

"The requested minimum move or angle for cutter compensation could not be made safely, cutcom statements were output with available engage and retract moves".

 

The problem is the combination of the min move in non-cutting moves and the min. move for comp on are more motion than there is space allowed.

 

First try taking the minimum clearance setting in non-cutting moves and set it to none. This may effect the switching to closed area engages type, so beware.

 

You can spend a good deal of time messing around if you truly want say... an arc on approach. But if you really just want to "not see the message" and you have some space to call comp on.

I'd change the engage to line, make the length zero. keep the height setting and set the comp move low like .005-.01.

This kind of makes the comp on-off motion your engage-disengage.

 

The message is usually OK. It's just telling you that you may not be getting everything you asked for.

It does not fit in that space.

It will put out the comp calls where they should work.

But I like you will often change my approach so I don't see the alarm.

 

Depending on your post, 1 out of 10 times the machine won't like where the comp gets put in and you will get an overcutting message at the machine.

 

Hope this helps, Paul S.

{Paul Schneider}, {CNC Programmer}, {DRT-Rochester}


Production: {NX11.0.2,MP5, NX12.0.1, MP2}

Re: Cutcom issues NX9 milling

Legend
Legend

Another last resort I sometimes use is the old cutter comp UDE. Check your code and make sure you get the results you are looking for, and that your register # matches etc...

 

When using this UDE, set the cutter comp on the ("non-cutting moves" > "more") tab to none.

 

 

cc ude 2.PNGcc ude 1.PNG

Glenn Balon
Production: NX 12.0.1.7 MP1 Primarily CAM

Re: Cutcom issues NX9 milling

Creator
Creator
Hi Glenn,

Yes, I have tried this and it has worked, I fully understand and we also use Vericut so can analyze NC path and gouging from there.

Thanks

Matt

Re: Cutcom issues NX9 milling

Creator
Creator
Hi Paul,

I also tried this and got pretty much exactly the results you stated. The machine reads the program fine for that particular part, it is good to have a few options as the components can vary wildly.

Thanks

Matt

Re: Cutcom issues NX9 milling

Creator
Creator
Hi Glenn,

I cannot seem to find this function on NX9, also as I am still relatively green to NX I don't fully understand UDE. I will however look more in to this and appreciate the thought and effort.

Thanks

Matt

Re: Cutcom issues NX9 milling

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

UDE = user defined event

In the operation, under "Machine Control" block -> Start (or End) of path events

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: Cutcom issues NX9 milling

Creator
Creator
Oh Ok,

Yes, I use Start and End events for adding BLK FORM and table movements.
This is basically manually adding cutter comp to a specific operation?

So I can do a single event for comp on and off in a specific operation?

Re: Cutcom issues NX9 milling

Legend
Legend

Yes, you can place the cutter comp UDE in the "start of path event." 

 

You can even select multiple operations and right click>object>start events. Beware this will alter any existing UDEs tied to that operation. 

 

 

I use this as a last resort though. Most users do not use it, and it can get messy having all those UDEs. 

 

I use it most on thread milling. Sometimes I have the perfect path, but the cutcom does not output where I want, so I use this UDE.

 

 

cc ude operation.PNGcc ude 1.PNG

Glenn Balon
Production: NX 12.0.1.7 MP1 Primarily CAM

Learn online





Solution Information