Change tool number without changing speeds and feeds

[Programinator]

Hello,  is there any way to change the tool number of a tool without it updating the feeds and speeds associated with that tool?  I know you can use the right click renumber tools or check the box in configuration to lock feedrates.  Sometimes i have 2 or more toolpaths with the same tool but certain toolpaths the feed or speed is adjusted.  Sometimes i want to change the tool number because the tool is already in the machine under a different tool number.  So if i go to the tool edit tool page and change tool, length, and diameter to a different number and update it changes all the feeds and speeds of all the toolpaths with that tool.  So any of the adjusted toolpaths feeds and speeds are erased and updated which i do not want.

Any way to avoid this without using lock feedrates or right click renumber tools?

thanks

 

[crazy^millman]

9 minutes ago, Programinator said:

Hello,  is there any way to change the tool number of a tool without it updating the feeds and speeds associated with that tool?  I know you can use the right click renumber tools or check the box in configuration to lock feedrates.  Sometimes i have 2 or more toolpaths with the same tool but certain toolpaths the feed or speed is adjusted.  Sometimes i want to change the tool number because the tool is already in the machine under a different tool number.  So if i go to the tool edit tool page and change tool, length, and diameter to a different number and update it changes all the feeds and speeds of all the toolpaths with that tool.  So any of the adjusted toolpaths feeds and speeds are erased and updated which i do not want.

Any way to avoid this without using lock feedrates or right click renumber tools?

thanks

 

You asking for a method that I am not aware you can do without using the lock feed and speeds what it was made for. The only way would be to have copies of the same tool in a file, but that would become a nightmare to manage IMHO.

[Programinator]

I don't like to work with lock feedrates on.  so for me to use that It would be a pain to go and change it just to change tool number, and then go change it back.  Would be nice if when changing a tool number a dialog pops up asking you if you want to update feeds and speeds or not.

[Tim Johnson]

You can have as many speed and feed versions of the same tool as you want. Copy the original tool, adjust speeds and feeds as needed then save the tool with either the changed feed/speed or as what process that tool is created for.

[Matthew Hajicek - Singularity]

I used to feel the same way, but have recently started working with the lock on.  You can always right click on the tool and reset to the tool's parameters, which I use for drills and reamers.  For everything else I use a speed and feed calculator to get the optimized parameters for each cut, as they're almost always different, so the parameters saved with the tool are irrelevant. 

[huskermcdoogle]

1 hour ago, Matthew Hajicek™ - Conventus said:

For everything else I use a speed and feed calculator to get the optimized parameters for each cut, as they're almost always different, so the parameters saved with the tool are irrelevant.

This is the most efficient way to make production parts and is how I have always operated.  You leave a lot on the table if you just run with defualts.  Especially when running dynamic roughing paths. 

I hate working with files that have 15 of the same tool because there were that many needed to manage feeds and speeds.  Just seems aweful messy.  When I make an endmill I set the speeds and feeds in the tool file for the generic side milling application parameters in say a generic alloy steel, and then adapt that per what I am doing with it on the files I use it on.

[Programinator]

My problem is this:  say I have a 1/4 endmill and the toolpth is finishing a 3 inch boss.  So for that I would just use the speeds and feeds associated with that tool.  I have my tools organized for materials as far as the feeds and speeds go.  So I can just open tool file for specific material and the speeds and feeds are generally good.  But then I use that same tool to do a 3/8 hole which would need to be slowed down.  So I just change the feedrate in the tool path parameters under the tool section. 

So I work remotely and after the programming in Mastercam I send the file to the shop and that's the last I see it.  Sometimes the guys at the shop want to change tool numbers for specific tools. So when they do that it changes that adjustment I made for the 3/8 día hole.  Then I get feedback saying my speeds and feeds were way too fast.  I could tell them to turn the lock feedrates on but the Mastercam users there don't like that on and I understand why.  I don't either. 

 

So I'm trying to figure out how to avoid that situation. 

[Leon82]

You could set it in the finish pass feed rate also.

 

[JParis]

Am I misunderstanding something?  This looks to be done quite easily...

I do not have lock speeds & feeds checked

 

[Leon82]

I believe since the costomer doesn't use lock feed rates, when the customer clicks the tool to change it's number it will default to the stored feedrate.

 

[JParis]

9 minutes ago, Leon82 said:

I believe since the costomer doesn't use lock feed rates, when the customer clicks the tool to change it's number it will default to the stored feedrate.

 

and that's exactly what the video shows..., I was thinking I was missing something maybe

[Guest]

On 1/17/2020 at 9:56 AM, Programinator said:

Hello,  is there any way to change the tool number of a tool without it updating the feeds and speeds associated with that tool?  I know you can use the right click renumber tools or check the box in configuration to lock feedrates.  Sometimes i have 2 or more toolpaths with the same tool but certain toolpaths the feed or speed is adjusted.  Sometimes i want to change the tool number because the tool is already in the machine under a different tool number.  So if i go to the tool edit tool page and change tool, length, and diameter to a different number and update it changes all the feeds and speeds of all the toolpaths with that tool.  So any of the adjusted toolpaths feeds and speeds are erased and updated which i do not want.

Any way to avoid this without using lock feedrates or right click renumber tools?

thanks

 

It seems to me lock feedrates is what you want, It is the path of least resistance IMO.

[Programinator]

3 hours ago, Leon82 said:

I believe since the costomer doesn't use lock feed rates, when the customer clicks the tool to change it's number it will default to the stored feedrate.

 

This is exactly the problem.  Same thing happens if you go to tool manager and change it from there. It just makes me look bad to the customer.  And for a remote worker that is not good.  I need my work to be near flawless because it's hard to defend myself from 100's of miles away. 

[Leon82]

2 hours ago, Programinator said:

This is exactly the problem.  Same thing happens if you go to tool manager and change it from there. It just makes me look bad to the customer.  And for a remote worker that is not good.  I need my work to be near flawless because it's hard to defend myself from 100's of miles away. 

If they select the ops and right click, renumber the tools I think the feeds will still be ok.

 

 

[huskermcdoogle]

5 hours ago, Leon82 said:

If they select the ops and right click, renumber the tools I think the feeds will still be ok.

If you do it like JP did I think they stay the same as well...  You just can't do it by editing the tool either in the tool manager or inside an operation.

I don't understand what the issue with lock feedrates is.  It's easy to pull the feed's and speed from teh tool if you have it, yes it is an extra click every now and again, but you never have to worry about losing your feeds and speeds.

 

Another thing you could do is use arc feedrate modification % when using contour 2d to reduce the feeds when doing a hole with a large tool.

[Programinator]

Thanks for all the ideas.  i think i will just have to encourage them to use the jparis method.  I just wish any method used would prompt you to pick if you want to keep speeds and feeds or replace with default in tool parameters.  

[Elmer Fudd]

On 1/17/2020 at 7:56 AM, Programinator said:

right click renumber tools

Doesn't this do what your looking for?  Anytime I need to change tool numbers this is what I do. It shouldn't change anything as far as speeds and feeds or step over or step down.

[JParis]

6 minutes ago, Elmer Fudd said:

Doesn't this do what your looking for?  Anytime I need to change tool numbers this is what I do. It shouldn't change anything as far as speeds and feeds or step over or step down.

You are absolutely right, it should...

I think what his offsite people are doing though, they are clicking on the tool.....and if lock speeds & feeds is unchecked that will reset the speeds and feeds...

At the end of the day, they need to be taught how to properly renumber tools IMHO

[crazy^millman]

23 minutes ago, JParis said:

You are absolutely right, it should...

I think what his offsite people are doing though, they are clicking on the tool.....and if lock speeds & feeds is unchecked that will reset the speeds and feeds...

At the end of the day, they need to be taught how to properly renumber tools IMHO

Yes and as a remote programmer I understand his frustration. End of the day hard to control things that we cannot control no matter how hard we try if there is a human involved on the other side we can never say 100% it will be correct. We can only do our best and cross the T's and dot the I's as best we can and go from there. I was going to make many of the suggestions made here, but seeing how I am called the meanest person on here some times I refrained. Press on and come up with some suggestions and examples and send them to QC and see what they say. 

[JParis]

15 minutes ago, 5th Axis CGI said:

Yes and as a remote programmer I understand his frustration. End of the day hard to control things that we cannot control no matter how hard we try if there is a human involved on the other side we can never say 100% it will be correct. We can only do our best and cross the T's and dot the I's as best we can and go from there.

As do I Ron, as do I....

[Bill Craven]

Sometime when I am programming remotely, I will create a level and add Drafting Notes for revisions and other things that they need to maintain awareness on.

For a couple of customers, I have a disclaimer about how changing tool numbers might change feeds and speeds.  

Then I set this as a Viewsheet and save it with that viewsheet as primary.  When they first open it, They will see it.  (they may not read it, and they may save it with a different screen)

Basically: I am covering my assets

[crazy^millman]

27 minutes ago, Bill Craven said:

Sometime when I am programming remotely, I will create a level and add Drafting Notes for revisions and other things that they need to maintain awareness on.

For a couple of customers, I have a disclaimer about how changing tool numbers might change feeds and speeds.  

Then I set this as a Viewsheet and save it with that viewsheet as primary.  When they first open it, They will see it.  (they may not read it, and they may save it with a different screen)

Basically: I am covering my assets

You should see our terms and conditions for some customers. For most it is 4 lines for others it maybe 20 to 50 lines.

[huskermcdoogle]

On 1/21/2020 at 4:50 PM, 5th Axis CGI said:

You should see our terms and conditions for some customers. For most it is 4 lines for others it maybe 20 to 50 lines.

Our contract is pretty solid...  Basically says the minute you get it from us it's your problem.  That said, we do everything we can to help them make a project successful.  We just can't be responsible for a machine crash, bad CAD geometry, forgotten features, poorly written posts, lack of properly vetted Vericut machine sim, or for lack of properly checking programs prior to running them on the machine.

Some customers lean hard on me to do everything for them, but understand that it is their rear on the line if something goes sideways.  Others, I don't have to life a finger after I hand them a Mastercam file, just need to show up and watch it run so I can take notes and make corrections or improvements where needed.

I typically find it takes about a week of working with a new shop to get them comfortable with em and myself comfortable with their individual capabilities both in the programming office and out on the shop floor.  After that working remotely on a project goes pretty smooth.  But the truth I have learned is that you always have to be flexible and adapt to the individual needs of each customer and understand what you can and can't do.

[Bill Craven]

14 hours ago, huskermcdoogle said:

I typically find it takes about a week of working with a new shop to get them comfortable with em and myself comfortable with their individual capabilities both in the programming office and out on the shop floor.  After that working remotely on a project goes pretty smooth.  But the truth I have learned is that you always have to be flexible and adapt to the individual needs of each customer and understand what you can and can't do.

I totally agree with this.  

I also do as much as I can to empower the machinist running the machine.  (including showing them the scars on my hands from running machines for years)

I need them as allies to be my eyes and ears to help improve the process.  

[Steelab]

On 1/19/2020 at 4:08 AM, Programinator said:

  Sometimes the guys at the shop want to change tool numbers for specific tools. So when they do that it changes that adjustment I made for the 3/8 día hole.  Then I get feedback saying my speeds and feeds were way too fast. 

If the guys running the machine want to change the tool number why do they need to go into Mastercam?...

 

Just open the G Code in notepad and Edit>Replace All>T(x) for T(y)

 

The only change will be the tool callout in the program, no need to re post or even open anything in Mastercam...

 

edit: one challenge with this method is if there is another T(x) in the program, for instance on our router there is a G500 T20 F32 in the beginning of the program so if I'm changing tool 2 to something else I need to make sure to change T20 back after adjusting the tool number...