Adjust feed rate at radius.

[PaulR]

Hello

 

I would like to adjust my feed rates when the tool transitions thru a radius. How do I do this?

[Josh T™]

Toolpath Editor

[PaulR]

Sorry, but can you be more specific?

[spade117]

Machine group properties > tool settings > adjust feed on arc move

[Josh T™]

Right click on the toolpath that you want to change - Select the Toolpath Editor (usually at the bottom of the list) - you can graphically change several parameters (i.e. feedrate). Just scroll through the position points and adjust what you want.

 

Hope this helps,

Josh

[NOTW Programmer]

This work great, it beats having to change at point. It is essentially the same principle only that the interface is more user friendly and not as confusing as change at point. Give this a try you'll love it !!

[David Colin]

But if you alter geometry and need to regen... you can't. So you must edit every point again. I really avoid to change nci data like that.

It'd be great if CNC system could implement an auto slow down/up before arcs and direction changes...

[Dave.L]

quote:

---

It'd be great if CNC system could implement an auto slow down/up before arcs and direction changes...

---

It sure would.

[Chris In-House Solutions]

Just a thought but have you played with the highfeed option. It doesnt let you input the feedrate you want the tool to roll around the corner at but will speed the tool up and slow the tool down based on the parameters you enter and the volume of material remaining on the part.

[peon]

The highfeed option also has a tendency of NOT retracting at the end of the toolpath, therefore, crashing through your part when starting the next toolpath if using the same tool. BE CAREFUL.

[cunder]

I like the settings as Spade says but I wish the option was in each operation rather than the machine group.

[kunfuzed]

Enhancement needed here!!!

[Scott Nordby - Form Tools Inc]

This has always been an issue for us. Machine group does not work. This is how we have fixed it. I added a couple lines to my post and use Misc real 4 and 5 to control it.

** add at the end of "parc"

code:

---

if arcrad$ < (tldia$ *2),

[

if mr4$ <> 0 & arcrad$ < ( tldia$ / 2), feed = feed * mr4$

if mr5$ <> 0 & arcrad$ > ( tldia$ / 2.001), feed = feed * mr5$

]

---

MI4$ is for arcs moves smaller than 1/2 the cutter dia.

MI5$ is for arc moves greater than 1/2 but less than 2 times the tool dia. (you can make this larger if you want but 2 times works well for us)

you can enter the percentage of change for each operation this way.

Hope this Helps

Scott

[Scott Nordby - Form Tools Inc]

Sorry for the miss spelling

should have been MR4$ and MR5$

---------------------------

MR4$ is for arcs moves smaller than 1/2 the cutter dia.

MRI5$ is for arc moves greater than 1/2 but less than 2 times the tool dia.