Rapids, Setting, speed?

[steveripplingerjr]

Can someone tell me where I can adjust my rapids speed? 

Does it automatically detect when it can use rapid movement? 

[jeff.walters]

when you generate a toolpath the yellow moves are done at a rapid. 

[fonsecr · Accepted solution]

By rapid we mean move as fast as possible on the particular CNC. So there is no feed setting for this one.

Usually rapid motion is mapped into G0 for ISO controls. However, occationally rapid gets mapped to feed moves using G1's. In this case the high feed needs to be specified but this is done during post processing - the post dialog has a property list which allows this depending on the post you use. In some cases the high feed might also be hardcoded when it is undesired to have to specify it.

[steveripplingerjr]

Yes that explains it a little more in depth. thanks! I'll check it out. 

[DESUDESIGN]

Same question here...How can we change the rapid movement rates?

[fonsecr]

Rapid are used for repositioning as fast as possible without engaging the cutter. The post will generally map rapids to G0s for ISO posts (sometimes G0s are forced to G1s for specific posts due to dogleg motion for the particular CNC).

In some cases it can be useful to manually use feed moves instead of rapids per toolpath operations or per NC program. For an operation you can use the high feed mapping on the linking tab. For the NC program you can change the high feed under properties in the post dialog.

René

[Steinwerks]

---

@DESUDESIGN wrote:

Same question here...How can we change the rapid movement rates?

---

If you really want to change your rapid (G00) move ratess, that is a machine setting and has nothing to do with CAM.

[DESUDESIGN]

We're running a Hurco mill. In post all of what should be G0 is coming out as G1. As a result, our "built in high feed rate" is limited to 300. To clarify, our yellow lines (rapid movements) should be G0 but are coded as G1. Way too many to tweak one by one in the code. There seems to be something in the Hurco Post that changes the Rapids to G1.

[fonsecr]

This would be by design.

HURCO can run in 2 modes: ISNC (ISO NC mode) and BNC (Basic NC mode). By default ISNC mode is used but you can switch to BNC mode by disabling the 'isnc' property.

HURCO does NOT synchronize the axes in ISO NC mode for G0s so the post will map these to G1s using the provided high feedrate when posting.

I guess we should update the post though so G0s are used when only a single axis is used.

René

[Steinwerks]

@fonsecr

Why does the HSM team insist on making decisions for users? At least do as has been done in the Haas post (only recently I might add) and add a 'useG0' option with a warning.

I had to edit our Fadal post in order to get it because no one at Autodesk would. I know what the machine does, and I plan for it. Stop hamstringing customers.

[DESUDESIGN]

Ah, that worked. Thanks!

[fonsecr]

To avoid machining crashes in this case. It is very common issue from experience.

The expectation needs to be that the CNC moves along the same path as has been simulated in CAM. So our posts are configured to use the safe behavior to prevent crashes.

That said, we do continuously update posts with new unsafe features that the user can tweak behavior. But these remain turned off by default. The most used posts get the most focus in general since there are a lot of post features that could be added. Post team will surely remain busy.

We have a lot of users from novice to experienced. And we cant assume that all users know what their CNC does. We try to set a reasonable bar on a per post basis, though.

René

[fonsecr]

Note that ISO NC and Basic NC modes are not compatible. E.g. drilling canned cycles are very different. So you cannot in general run ISO NC program in Basic NC mode in the CNC and vice versa.

René

[fonsecr]

Updated ISO NC mode to use G0 when only a single axes is moving.

https://cam.autodesk.com/posts/?p=hurco
https://cam.autodesk.com/posts/?p=hurco3d

René