Showing results for 
Search instead for 
Do you mean 
Reply

Spindle speed change automatically when change cutter

I copy a program and change the cutter . The Spindle speed change automatically. It is quite often . Is there any setting that can change this setting?

Attached is the file for reference.

3 REPLIES

Re: Spindle speed change automatically when change cutter

Assuming the 2 tools have different diameters...

It looks like the operation is using the "surface speed" (smm) as the "master" data, and changing the RPM as needed to satisfy the SMM specified for that diameter tool.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Spindle speed change automatically when change cutter

Hello @Edwin_DTS

 

We have seen this also usually when changing two of the fields it forces you to use the recalculate button that then updates Spindle Speed, Feed, Surface Speed and Feed Per Tooth the main issue we have with this is that it can change the spindle speed to above the Max available and sometimes that section auto closes so it is not always picked up until posting where we have added a check to alert the user.

 

When I asked GTAC it was deemed as working as designed?

 

 

Regards

Dave
NX10.0.3MP13
NX11.0.1
Production
TC10
Vericut 7.3,7.4.1,8.0.2

Re: Spindle speed change automatically when change cutter

It has had these issues all the way back to 7.5 or further.

Many have complained and no change...

 

I like how you set the speed and feed. See the values, OK the process and it tweaks the spindle speed a little

If you have any OCD you have to go back in and edit again. Usually fine then.

 

Really want a good time try to program as IPR (without a special post)

 

As a great review tool I turn on the speed and feed columns in the feature navigators

(right click the column header and choose.. columns...configure, it is at the bottom) Then I can see issues at a glance before posting.

* See picture *

 

I have often found it easier to change both speed and feed by right clicking one or multiple process and going to Object.. Feedrates and changing here. Especially helpful to edit in the tool navigator to grab all processes for that tool and set the same in one move

 

*** If you grab multiple process and the first one has a speed and feed (doing the object... feedrates, edit) without changing anything, you just hit OK to your edit. All the proceeses will inherit the first processes speeds and feeds.

***Same thing can be done to with start events and end events to get multiple processes to inherit the same start and end events

 

Lastly if you do not tab thru the boxes when the dialog is open, but mouse pick them... it will not prompt for a recalculate you can edit both and the "OK" button will not gray out, forcing the recalculate.

 

Hope these notes are helpful, Paul S.

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


Production: {NX11.01, SP2}

Learn online





Solution Information