grouping or combining toolpaths

[Doug Funny]

Greetings All,

Is there a way to group multiple toolpaths into one toolpath or group? For example, spot drilling. If I have several spot drill toolpaths and I want to combine them into one toolpath so, I can optimize X,Y positions and have it change z depths instead of bouncing around from one set of holes to another?

 

TIA Doug

[AHarrison1]

In Linking Parameters Set as follows

Clearance - Absolute  - Initial Z usually above top of stock

Retract - Incremental Z distance above selected point

Top Of Stock - Incremental Z height position of point

Depth - Incremental Z depth from selected point If all holes are the same depth

 

[Doug Funny]

23 minutes ago, AHarrison1 said:

In Linking Parameters Set as follows

Clearance - Absolute  - Initial Z usually above top of stock

Retract - Incremental Z distance above selected point

Top Of Stock - Incremental Z height position of point

Depth - Incremental Z depth from selected point If all holes are the same depth

 

Thank you, is there a way to handle holes at variable depths? What I've been doing is going into my geometry and manually setting depths. This does what I want but, it can be time consuming

[TFarrell9]

11 minutes ago, Doug Funny said:

Thank you, is there a way to handle holes at variable depths? What I've been doing is going into my geometry and manually setting depths. This does what I want but, it can be time consuming

Use incremental values and check the "calculate depth from top of stock" box under the "depth" box.

[AHarrison1]

The above would be 1 scenario where you have holes on various Z levels but all the same depth.

Scenario 2 Same size diameter holes on the same Z level but with different depths then pick the bottom of the holes

Clearance - on or off makes no difference

Retract - Absolute Z distance above selected point

Top Of Stock - Absolute Z 0

Depth - Incremental Z 0 (or minus a little for drill point

If Different Diameter holes then it will be different ops

[Leon82]

Sometimes you can use absolute top of stock with incremental depth for they are different depths from one plane. 

 

You can also make toolpath sub groups that would house each tool

[cruzila]

Do you wan to use one G81 with multiple Z? Some machines may not support this.

[Leon82]

20 minutes ago, cruzila said:

Do you wan to use one G81 with multiple Z? Some machines may not support this.

I think he's more interested in doing multiple holes with one mastercam op

[crazy^millman]

I have a crazy suggestion. How about making a sample file that represent what you are trying to accomplish. Then others can use that file to give you different suggestions. If others are wondering the same thing then they can also learn from this thread. Don't forget about solid holes as features that can used

[Jespertech]

This is kind of on topic but not really, but it's an approach that works well for me that others might find helpful, or perhaps I'll find a better way through sharing this.

Usually  I'll create sub groups within my spot drill cycle and label them for each set of holes. 

for example I have 4, 3/8-16 tapped holes on the face of my part and 6, 1/4-20 tapped holes at the bottom of a C-bore. 

That way when I go to create the drilling cycles all I have to do is copy and paste the specific toolpath then change the tool and parameters and I'm done.

I'll then do the same for the tapping cycle.

This has improved my workflow and programming time quite a bit in parts that have a lot of different hole features. 

 

[Chally72]

Have any of you played with the Chamfer Drill toolpath to do spotting on dissimilar holes or groups of holes? This will allow you to enter a positive or negative number for chamfer depth, and automatically adjusts SFM for different hole sizes. So if I wanted to do something like spot 4 holes of 4 different diameters to a spotting diameter of (Ø - 0.020"), you could do this with chamfer drill and have variable depths on variable hole sizes, with variable speeds, all in a single operation.

[#Rekd™]

Just now, Chally72 said:

Have any of you played with the Chamfer Drill toolpath to do spotting on dissimilar holes or groups of holes? This will allow you to enter a positive or negative number for chamfer depth, and automatically adjusts SFM for different hole sizes. So if I wanted to do something like spot 4 holes of 4 different diameters to a spotting diameter of (Ø - 0.020"), you could do this with chamfer drill and have variable depths on variable hole sizes, with variable speeds

Any chance you could provide a sample file or a video on this?

[Chally72]

Check out the attached sample file- 3 different hole sizes, all spotted using a 142° tool in a single toolpath.

Here you see the different depths we drive to on each size:

On the three different holes:

And because we checked "Maintain SFM", we get spindle speed drops as we go up in hole size:

Sample Spotting.mcam

[Radical1]

I have never noticed this toolpath before, this is the best! I see it does not do the G81 which would make the code a bit longer but a pretty good trade off.

[Radical1]

On another note, as I played with the settings in the sample file I realized I really miss the "refresh toolpath" button in M/C 2023.

Bring back the refresh!!!

[Chally72]

Radical, do you mean the Preview toolpath button that used to live on the top toolbar of a toolpath dialog? 

 

That's been merged with the Apply button (Blue Plus) next to the green check and red X. So, Apply is really now "Apply and Preview" in 2023. Yes, this is super unclear and I hope we can make this more distinct in the future. Hope that helps!

[Radical1]

2 hours ago, Chally72 said:

Radical, do you mean the Preview toolpath button that used to live on the top toolbar of a toolpath dialog? 

 That's been merged with the Apply button (Blue Plus) next to the green check and red X. So, Apply is really now "Apply and Preview" in 2023. Yes, this is super unclear and I hope we can make this more distinct in the future. Hope that helps!

Thanks Dylan, I did not realize that. I don't use the apply button because with much earlier versions of M/C clicking the apply button caused the software to crash...now I know.

[crazy^millman]

5 hours ago, Chally72 said:

Check out the attached sample file- 3 different hole sizes, all spotted using a 142° tool in a single toolpath.

Here you see the different depths we drive to on each size:

On the three different holes:

And because we checked "Maintain SFM", we get spindle speed drops as we go up in hole size:

Sample Spotting.mcam 490.81 kB · 4 downloads

Wow a Sample file and people can see what you are seeing and can ask questions about what you are doing.

Crazy I tell you.

[Doug Funny]

18 hours ago, crazy^millman said:

Wow a Sample file and people can see what you are seeing and can ask questions about what you are doing.

Crazy I tell you.

My apologies

[Doug Funny]

23 hours ago, Chally72 said:

Check out the attached sample file- 3 different hole sizes, all spotted using a 142° tool in a single toolpath.

Here you see the different depths we drive to on each size:

thank you Chally72, this is is kind of what I'm looking for but, what if you want a different size chamfer on each hole?

Say the first hole you want a .02 chamfer, the second you want .05 and the 3rd you want .075. Is there a way to accomplish this in a single operation?

I'm trying to avoid tools from going from one end of a long part to the other and back again spotting or chamfering holes with different chamfer size requirements

[crazy^millman]

16 minutes ago, Doug Funny said:

Wow a Sample file and people can see what you are seeing and can ask questions about what you are doing.

Crazy I tell you.

My apologies

No need to apologize. Sorry I just don't understand why it is so hard to put together a sample file so you have something to reference. I go into shops to train programmers from time to time. I take a part they are struggling with and I teach them how to program it. We then go over the RMB, configuration settings and other things. Now they have more than some book lesson or blog posting. They have a real world example of what it takes to get it done. That is all I am trying to give you here is something when you are not sure you could always go back and reference. I have 242 files in my Emastercam Dropbox folder of different files I have helped people with over the last 10 years. I have maybe 500 files in the my different shared Mastercam version saved also. I have experience because I seek it and learn from others. For you to get experience get out of your comfort zone and be willing to use the resources you have. This is one of them so make up a sample and now you got something you can learn from.

Go to CAMinstructor and download my 5 Axis model and review Ron Week. I put a lot of time and effort into making that block to help others. I had a bone to pick with a company that was trying to make me change my company name. I also wanted to show others how you can work with only a solid for programming in Mastercam. I have always been willing to put my money where my mouth is. I make mistakes just like anyone. I do dumb things also. Part of learning and getting better at this profession.

[crazy^millman]

3 minutes ago, Doug Funny said:

thank you Chally72, this is is kind of what I'm looking for but, what if you want a different size chamfer on each hole?

Say the first hole you want a .02 chamfer, the second you want .05 and the 3rd you want .075. Is there a way to accomplish this in a single operation?

I'm trying to avoid tools from going from one end of a long part to the other and back again spotting or chamfering holes with different chamfer size requirements

Yes model the part with the different chamfers. Then you use chamfer and grab the upper edge of the chamfer and tell it you want a .001 chamfer. Then in the stock to leave on the wall you tell it to leave .001. Now the chamfer tool path will cut every chamfer no matter the size exactly how it is modeled. Where knowing solid modeling methods are a huge time saver in programming. Before we got the method we have now I might have to revolve a chamfer or use solid model sweep to create them. I have even modeled them as surfaces and then came back and made the surface model a sheet solid.

[Chally72]

Just a note that Zero is a valid size for chamfers in Chamfer Drill, so you don't have to use Ron's method to get the physical chamfers you want. Different chamfer on each hole? Model them all in. Same chamfer on different holes? You don't have to model them in to get what you need.

Chamfer drill was designed for these scenarios- to allow a single op to tag all sorts of different modeled chamfers, or to allow you to specify a chamfer size if the chamfers weren't modeled in. The spotting method is kind of a hijacking of it since you aren't technically producing a Chamfer, but I use it all the time to condense my spotting operations when I don't have to get too picky with spot size across a range of diameters.

[#Rekd™]

Dylan do you have anything on the advanced drill tool path, a video or a sample file?

Thank you for all of your help!!!

 

[Doug Funny]

1 hour ago, crazy^millman said:

Yes model the part with the different chamfers. Then you use chamfer and grab the upper edge of the chamfer and tell it you want a .001 chamfer. Then in the stock to leave on the wall you tell it to leave .001. Now the chamfer tool path will cut every chamfer no matter the size exactly how it is modeled. Where knowing solid modeling methods are a huge time saver in programming. Before we got the method we have now I might have to revolve a chamfer or use solid model sweep to create them. I have even modeled them as surfaces and then came back and made the surface model a sheet solid.

I modeled the appropriate chamfers and used a Chamfer Drill operation. The only downside is that Chamfer Drill long codes everything out instead of using canned cycles. Most of the machinist here are a bunch of old curmudgeons. If the see programs like this, I'll never hear the end of it.  Is there a way to get Chamfer Drill to output a canned cycle?