SlaveCam

Circle Mill, no starting diameter for roughing?

Recommended Posts

The case: drill a hole and make it bigger with a circle mill. The drill diameter is 16 and the desired hole diameter 20 and the endmill is 10. How do I make the circle mill start roughing so that it won't cut air?

 

Thanks!

Share this post


Link to post
Share on other sites

use semi rough and calculate the difference between holes/2 then set up # of cuts and distance.

 

Just did that today...

  • Like 1

Share this post


Link to post
Share on other sites

2d dynamic

Desired hole is machining geometry

Starting hole is Air

Works really well

  • Like 4

Share this post


Link to post
Share on other sites

2D Dynamic :w00t:

Share this post


Link to post
Share on other sites

2d dynamic

Desired hole is machining geometry

Starting hole is Air

Works really well

 

Wish I'd thought of that before!    Did they have that option in X8?   I know they didn't in X7

Share this post


Link to post
Share on other sites

Wish I'd thought of that before!    Did they have that option in X8?   I know they didn't in X7

 

Air regions was new to X9. It is a really nice addition to the HST toolpaths. Just have to remember to set the outside in the settings. When it is set to inside then the air regions will be ignored. It can be a little confusing if you are cutting from the inside of a part. The outside and inside are referring to the cut pattern itself. Does the toolpath need to stay inside the containment boundary or is it allowed to start outside the toolpath containment boundaries. Not sure how it could worded different to not confuse it someone that might be doing work inside or outside of a part they are cutting, but I have to say it took using it a little to see what this setting means and does to a toolpath, but trust me it can make a huge difference on the toolpath. I was cutting a 100" diameter forging. It took 16 hours to rough it using inside. I then switched it to use outside thanks to Dave Conigliaro point out I made the mistake and it only took 8 hours hours to rough the next part by switching it to outside.

 

Also have to be careful if you are using solids for your toolpath any changes to the solid and you loose all your chaining. I know the solids are meant to make not having to create geometry for the toolpath the process, but I have a part that has had 5 rev changes on it and I have been using the Model Prep to bring the programmed part to that level. All toolpaths that were not effected by the change had their chains erased. In hindsight it would have been better to just make chains, but I didn't expect the customer to make so many rev changes so it is what it is. Think about that is only using Solids to drive your HST toolpaths. I have not tested it, but I think Mastercam for Solidworks handles this differently. You make changes to the solids and the association to feature not effected by the model change are made dirty, but not erased.

  • Like 1

Share this post


Link to post
Share on other sites

I'm still waiting for this feature. How come we still don't have it, considering how useful it would be? Dynamic toolpath is a much more heavy operation that can do it, but I prefer to use "light" operations whenever possible with no additional geometry.

Share this post


Link to post
Share on other sites
6 hours ago, SlaveCam said:

I'm still waiting for this feature. How come we still don't have it, considering how useful it would be? Dynamic toolpath is a much more heavy operation that can do it, but I prefer to use "light" operations whenever possible with no additional geometry.

Circle mill most likely will not recieve much attention especially considering there is a viable alternative.

  • Like 1

Share this post


Link to post
Share on other sites
On 9/10/2021 at 1:29 PM, cncappsjames said:

Circle mill most likely will not recieve much attention especially considering there is a viable alternative.

Agreed, also I have found that 2D dynamic is just faster many times.

 

With that being said, I use Helix Bore operations quite a bit these days. You can basically do the same with a 2D ramp but this toolpath makes it mindlessly easy. Helix down, you can have multipasses if necessary and then you can have a fully customized finish pass all within the same toolpath. I feel like Helix Bore doesn't get the love it deserves.

A Circle Toolpath "refresh" from CNC software sure would be a nice thing tho....

  • Like 5

Share this post


Link to post
Share on other sites
On 9/10/2021 at 9:08 AM, SlaveCam said:

I'm still waiting for this feature. How come we still don't have it, considering how useful it would be? Dynamic toolpath is a much more heavy operation that can do it, but I prefer to use "light" operations whenever possible with no additional geometry.

Are you open to a 3rd Party Solution? The Circle Mill Nci could be edited to do what you want using a chook.

 

  • Like 1

Share this post


Link to post
Share on other sites
5 hours ago, Metallic said:

Agreed, also I have found that 2D dynamic is just faster many times.

 

With that being said, I use Helix Bore operations quite a bit these days. You can basically do the same with a 2D ramp but this toolpath makes it mindlessly easy. Helix down, you can have multipasses if necessary and then you can have a fully customized finish pass all within the same toolpath. I feel like Helix Bore doesn't get the love it deserves.

A Circle Toolpath "refresh" from CNC software sure would be a nice thing tho....

I do use Circle Mill and Helix bore because I often re-use operations and I can change a drilling op to helix/circle and as long as I picked the geometry with using the path in the future, it is 4-ish mouse clicks and done. But since they haven't shown it any real lovin' in a long time, I'm not holding out hope. :rofl:

Share this post


Link to post
Share on other sites
10 hours ago, Metallic said:

Agreed, also I have found that 2D dynamic is just faster many times.

Faster how? It it *much* slower to generate a 2D Dynamic toolpath than a Circle Mill for round geometry simply because 2D Dynamic uses a very complicated algorithm for the toolpath whereas Circle Mill is very simple, so much as I have made a radial helix macro as one of my custom drilling cycles for our Mazak's.

Circle mill is also simple to use, requires fever clicks, options to set and geometry to draw. For me, simpler is often better. The code generated is terse and fits in smaller machine's memory, no need to use filtering. There are alternatives yes, but surely the aim here is to be as productive as possible? Not to mention that semantically it makes sense to use Circle Mill for radial helix :)

10 hours ago, Metallic said:

I feel like Helix Bore doesn't get the love it deserves.

It does from me. It's the second most used operation after drilling in the parts I program. It's great for both finishing and roughing with a high feed mill. I've many times hoped for an Advanced Helix-Bore operation that would let me create segments of pitch, feed and other variables similar to Advanced Drill.

10 hours ago, Thee Kid™ said:

Are you open to a 3rd Party Solution? The Circle Mill Nci could be edited to do what you want using a chook.

 

Why can't you just add the "starting diameter" text box in the dialog with some DLL injection? 😎

Just kidding, don't do that. It's illegal

  • Like 2

Share this post


Link to post
Share on other sites
6 minutes ago, SlaveCam said:

I've many times hoped for an Advanced Helix-Bore operation that would let me create segments of pitch, feed and other variables similar to Advanced Drill.

+ eleventy billion

  • Like 1

Share this post


Link to post
Share on other sites
18 hours ago, SlaveCam said:

Why can't you just add the "starting diameter" text box in the dialog with some DLL injection? 😎

Just kidding, don't do that. It's illegal

I like your thinking! Hmmm, I wonder how long that would take to program? 

Share this post


Link to post
Share on other sites

Try this:

( as for first post in topic )

on roughing page - check helical entry, 

XY clearance = 2.2

Plunge angle = 0.0

Works for me

Share this post


Link to post
Share on other sites

I usually just do a little math and change the minimum and maximum radius values to accomplish this.  The other key is to set  your top of stock and depth both to the final z depth (obviously you can't to this if you plan on using z depths) and change your feed plane to the top of the hole so it feeds straight down to the cutting depth.  Also, set the Z clearance value in the Roughing parameters to 0.

 

pbGil17.png

 

c8lyxUl.png

 

XlB11YK.png

  • Like 1

Share this post


Link to post
Share on other sites
23 hours ago, Thee Kid™ said:
On 9/13/2021 at 10:36 PM, SlaveCam said:

Why can't you just add the "starting diameter" text box in the dialog with some DLL injection? 😎

Just kidding, don't do that. It's illegal

I like your thinking! Hmmm, I wonder how long that would take to program? 

So you would have to create a completely new menu for the operation with all the fields, the chook operation can override the parameters dialog even so a custom dialog appears then your starting diameter would appear there, the chook would always be needed to maintain the new parameter, otherwise the operation will revert to its original state.

The Nci editing would be the easy part, the ui is rather labor intensive, but thats kinda my thing!  :crazy:

 

Share this post


Link to post
Share on other sites
On 9/15/2021 at 8:35 PM, neurosis said:

I usually just do a little math

I like math but...no comments.

On 9/15/2021 at 11:23 PM, [email protected] said:

the ui is rather labor intensive, but thats kinda my thing!

To be honest, frontend sucks. If only I could do backend only and leave the ui to others (without switching jobs that is).

Share this post


Link to post
Share on other sites
On 9/13/2021 at 11:40 AM, Metallic said:

I feel like Helix Bore doesn't get the love it deserves.

This is my go to for circular paths...drive it with a point!

  • Like 2

Share this post


Link to post
Share on other sites
4 hours ago, SlaveCam said:
On 9/15/2021 at 4:23 PM, [email protected] said:

the ui is rather labor intensive, but thats kinda my thing!

To be honest, frontend sucks. If only I could do backend only and leave the ui to others (without switching jobs that is

What framework do you use?

 

Share this post


Link to post
Share on other sites

Hi guys, I've been away for a few days, don't go all conspiracy theory on me that these are dead products... We've made a lot of improvements to them in the past few years!  :)

 

SlaveCam - This is a good idea, I don't believe I've seen it mentioned before.   I was thinking through the parameters, but the easiest solution to me seems to just recognize stock, so I think that's the direction we're going to go with it..  That'll solve the problem of multiple sizes of holes selected at the same time and work the same way as the rest of the product.

Thanks for the good idea.  As a note, you'll probably get faster response from CNC if you either post on our forum or email requests like this into [email protected]

 

Cheers,

Share this post


Link to post
Share on other sites
5 minutes ago, Aaron Eberhard - CNC Software said:

but the easiest solution to me seems to just recognize stock, so I think that's the direction we're going to go with it..  

Seems to me that that would be mote computationally expensive than having a hole diametet of the drill.. 

  • Like 1

Share this post


Link to post
Share on other sites
19 minutes ago, Aaron Eberhard - CNC Software said:

Eh, cycles are cheap... And there's no guarantee that you used the same sized drill for a variety of hole sizes.

Yeah, I was speaking more to the specific case where the drill was all the same size, I think? Anyway I was hoping you would chime in, great to have a response from the p.o.

!

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us