Problem running posted programs from HSM VALUE EXCEEDS MAXIMUM

I have a Hurco VMX24 brand new machine 2018 model, I'm using Inventor HSM to create cad/cam programs, i have already edited the post processor to allow tool number, lengths and diameters to 999 for example (tool.lenght > 999) this was firstly preventing my programs from working correctly with the error code VALUE EXCEEDS MAXIMUM.

I now have the same error code even though all adjustments have been made, its a small job so cant be limits on the axis. I'm using Fanuc industry standard post processor. Anyone had this issue and managed to fix it?

I am new to cad/cam and only 21 so please bare with me.

You may also need to edit the post processor to account for max feeds/rapids.

Chazsani


Sent using CIMCO Edit DNC

LukeGernon said:

I have a Hurco VMX24 brand new machine 2018 model, I'm using Inventor HSM to create cad/cam programs, i have already edited the post processor to allow tool number, lengths and diameters to 999 for example (tool.lenght > 999) this was firstly preventing my programs from working correctly with the error code VALUE EXCEEDS MAXIMUM.

I now have the same error code even though all adjustments have been made, its a small job so cant be limits on the axis. I'm using Fanuc industry standard post processor. Anyone had this issue and managed to fix it?

I am new to cad/cam and only 21 so please bare with me.

Click to expand...

What tool number are you programing in your CAM and is the number higher than your tool capacity of your machine?

Are you getting the error at the in HSM or at the machine?

The default HSM post for Hurco ISNC makes all rapid moves feed moves...which can cause an error similar to yours (my machine is older and I don't remember the exact error), because the machine sees a feed move (G01 or G03 or G04) commanded at a feed rate above its max contouring feedrate.

Check and make sure that your "rapid feed" doesn't exceed the machine's max contouring rate.

I believe that HSM has the default post set up this way to avoid crashes with rapids on older machines like mine, as at least the older controls (not sure about the newer ones) do not force completion of one set of rapid moves before starting the next rapid move (ie X and Z rapids commanded followed by another X rapid, if first X rapid is completed before the Z rapid is completed it will continue straight into the next X rapid while the Z rapid finishes....can make for nasty crashes). So HSM opted to have the default all feed moves to avoid that problem. That's what I heard/read somewhere anyway.

On my machine max contour is 300ipm, rapid is 750ipm...makes for some slow programs when the rapids have to be 300ipm.

Hope that helps.

Leviathan

Sent from my SM-G930W8 using Tapatalk

my machine has tool numbers up to 1000 so this shouldn't be an issue. and have run programs using fanuc with high tool numbers before.

The error is on my machine control, I think it might be the feeds/speeds or rapids limits in the post processor what can I edit in the post to adjust this ?

Two places to check:

Under the settings for the specific machining strategy go to the "linking" tab (last one...far right). You are looking for high feedrate mode: default I believe is "preserve rapid movement"...on my machine none of these settings make any difference, because the post makes all rapids into feed moves anyway. But you can experiment with these settings...may work differently on your machine.

You are also looking for the "allow rapid retract" and the "no-engagement feedrate" make sure the no engagement feedrate is set to less than your machine's max contour rate (on the slowest axis) if this is set too high you will get that error.

Lastly when you go to post out check the post settings in the lower right of the post process dialog box. Check the setting for the high feed mapping (my understanding is that this will override the high feedrate mode I wrote about above). Then most importantly set the (built-in) "high feedrate" to your max contour feedrate...as this is the speed that the post will output in place of rapids.

Hope that helps...I have no idea how different the capabilities of the newer Hurco controls are in this respect...probably worth a call to Hurco and the HSM people if you will be using CAM for this machine a lot. For me the difference in run time is significant between conversational with 750ipm rapids vs CAM with 300ipm. Especially if it's simple drilling and tapping etc. Complex milling it's worth the slow down, but anything 2D milling the run time in conversational is much faster for just this reason. I would hope that a newer Hurco with a MAX4 or MAX5 control only needs a custom post to fix this issue. Though depending on your machine your max contour rate may be very close to the same as your rapid feed.

Leviathan

Sent from my SM-G930W8 using Tapatalk