Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Refugee from Fusion 360 looking for advice


RecceDG
 Share

Recommended Posts

5 hours ago, Metallic said:

I want to throw in my tidbit of guidance - I have given up completely on MCfSW in my applications. And I am in the education field, so I am always trying to find the EASIEST CAM transition for brand new students.

Well as a refugee from Fusion 360, one of the things that Fusion does well (enough) is the marriage between CAD and CAM. I'm very much used to having them both in the same place.

Back in my former life, Mike the Machinist ran MC Standalone and imported my parts out of SW. I see why he did that, but if I have the option to stick to one UI, I would prefer that.

The other thing Fusion is good at is the "one licence, run anywhere" aspect of the cloud. My primary design machine is in my basement, my lathe (and soon, mill) are in the shop in an outbuilding, and the CNC router is in the garage. I do most of my design work on the "design studio" machine, but it has proven to be *very* useful to be able to pull up Fusion at the machine (all my machines are PC driven) to make tweaks. Solidworks lets me do this, Mastercam only allows one installation per licence. I really wish I could install MC on all 3 machines, and have MC limit me to one *running* instance at once.

Link to comment
Share on other sites
On 8/13/2021 at 6:07 PM, RecceDG said:

Screengrab of planes manager. I mucked around setting various planes to WCS and T with the "=" button, but none of them fixed that chain.

Then I tried a groove operation, selecting the faces between the "tires" - so the big turn flat, the two fillets on each side of it, and the little tiny facing flat as the groove blends into the "tires" - and that worked!

So then I did a second groove op, this time on the "axle" and the "bell" radius, and it kinda worked, in that it correctly cut the "axle" and "bell", but to do so it plunged straight through the "tire".

It's like it doesn't see that part of the model - like the "tire" doesn't exist.

lathe_planes_2.png

groove_ok.png

groove_notok.png

The only WCS that you need to use for lathe is Top, all the other ones make a mess.  So, you set the model the way the part is going to sit on the chuck, create another level, and then do a Turn Profile.  That's all you need.

On 8/13/2021 at 6:07 PM, RecceDG said:

Screengrab of planes manager. I mucked around setting various planes to WCS and T with the "=" button, but none of them fixed that chain.

Then I tried a groove operation, selecting the faces between the "tires" - so the big turn flat, the two fillets on each side of it, and the little tiny facing flat as the groove blends into the "tires" - and that worked!

So then I did a second groove op, this time on the "axle" and the "bell" radius, and it kinda worked, in that it correctly cut the "axle" and "bell", but to do so it plunged straight through the "tire".

It's like it doesn't see that part of the model - like the "tire" doesn't exist.

lathe_planes_2.png

groove_ok.png

groove_notok.png

The only WCS that you need to use for lathe is Top, all the other ones make a mess.  So, you set the model the way the part is going to sit on the chuck, create another level, and then do a Turn Profile.  That's all you need.

Link to comment
Share on other sites
11 hours ago, RecceDG said:

Sent.

I gave you copies of both files.

The email was in my inbox this morning. I took a look and replied to your email.

I think you uncovered an issue with automatically generating lathe profiles from solids containing 180 arcs on them.

Pete

Edited by Pete Rimkus from CNC Software Inc.
  • Like 1
Link to comment
Share on other sites
  • 3 weeks later...
  • 1 month later...

So i checked the configuration of my rapids in Mach 4, and I had the Z at 90 in/min and the X at 20 in/min.

Those got bumped up to 175 in/min (!) and 35 in/min.

X I increased because at 20 in/min max speed, at higher spindle RPM I started knocking on feed/rev limits that I might actually use - which could be a problem if I was moving both axis simultaneously, like cutting a chamfer or a radius. I presume Mastercam has some place in the machine configuration that specifies max axis speeds, so I gotta go find those and set them correctly.

Another interesting question is - how fast (shaft RPM) can a steel screw be spun in a brass nut before wear becomes a concern? I haven't the foggiest idea of where to look that up. Textbooks on machine design? And I suppose threadform matters too.

Any ideas?

Link to comment
Share on other sites
1 hour ago, RecceDG said:

So i checked the configuration of my rapids in Mach 4, and I had the Z at 90 in/min and the X at 20 in/min.

Those got bumped up to 175 in/min (!) and 35 in/min.

X I increased because at 20 in/min max speed, at higher spindle RPM I started knocking on feed/rev limits that I might actually use - which could be a problem if I was moving both axis simultaneously, like cutting a chamfer or a radius. I presume Mastercam has some place in the machine configuration that specifies max axis speeds, so I gotta go find those and set them correctly.

Another interesting question is - how fast (shaft RPM) can a steel screw be spun in a brass nut before wear becomes a concern? I haven't the foggiest idea of where to look that up. Textbooks on machine design? And I suppose threadform matters too.

Any ideas?

Open the Machine Definition Manager and open the General Machine Parameters. You can set your min/max feed limits there.

Can't help with the steel screw brass nut info. I would think remaking the nut out of oil impregnated bronze might help.

Capture.PNG

Link to comment
Share on other sites

Brass is good for non stick as it's a dissimilar material.

But not for wear characteristics. Bronze is a better bet.....

Ref rapids - I'd be careful with too high - you don't want any galling on slideways or screws. Settle for what the machine is.....(no offence it's a cool project)

Link to comment
Share on other sites
3 hours ago, Newbeeee™ said:

Brass is good for non stick as it's a dissimilar material.

But not for wear characteristics. Bronze is a better bet.....

Ref rapids - I'd be careful with too high - you don't want any galling on slideways or screws. Settle for what the machine is.....(no offence it's a cool project)

Would Not Oil Impregnated Bronze  be a Better Choice for Wear Items IE like Swing Arm Bushings   and Other Rotational Items ? I have not looked up the Specs Just going off of some older replacement items on things that go around and around .??:scooter:

  • Like 1
Link to comment
Share on other sites

Given the construction of the Z axis, I think I'm OK cranking up the Z rapids - and honestly, with the duty cycle of this machine, there's just not a ton of time spent moving; it's not like the machine is running 24/7. But at the same time, speeding up my cycle times is nice.

The X rapids I'm way more hesitant about. Here, I'm not so much looking at cycle times, but making sure the axis is fast enough to keep up with 2-axis moves for chamfers or radii. At the slow speeds I had the axis set for, at faster spindle RPMs I was getting into max in/rev that I'd actually want to use (like 0.008"). Bumping the max speed up to 35 in/sec means I can do about 0.015"-ish in/rev at 3000 RPM which is more headroom.

As far as the nut goes, yeah, some SAE 660 bronze is probably a better alloy. It's a part I can make too, it's a cylindrical pin that fits into a hole in the carriage, cross-drilled and threaded. If I get a form tap I should be able to make a nice smooth thread.

*sigh* I thought I was done making lathe parts.

I really wish I could find some sort of formula or table that detailed max thread rotational speed by thread pitch, diameter, and material.

I also wish I knew how to calculate the force needed to drive a cutting tool into a part. What I have now is the most powerful stepper I could fit, geared down 1:2, and then the M10x1.0 leadscrew thread. The idea was to maximize the force the crosslide could generate so that the stepper would never stall - at the cost of rapid speed.

For a while, the limiting factor was the power of the spindle motor (so sometimes when parting I could stall the spindle) but that was largely an artifact of the fabricobbled spindle motor pulley, driving a metric belt with an SAE pulley. Once I cut my own motor pulley I appear to have eliminated belt-slip stalling, and now I suspect the torque limit is the 9mm GT2 X axis drive belt.

I wish I knew how to work out these forces from first principles, even as a rough approximation to see if I'm in the ballpark.

The lathe performs great, but parting off (although it has gotten much better) is always a bit of an adventure.

The sad truth though is that the underlying bar-bed design is just too flexy, and at some point, I'm just turd-polishing. I will eventually pick up one of these: https://www.kingcanada.com/en/products/metalworking/metal-lathes/kc-1236ml-12-x-36-gearhead-metal-lathe and convert it. Luckily, all my CNC-bits will port over.

 

Here's what 175 in/min Z and 35 in/min X looks like:

 

Link to comment
Share on other sites

It's a tradeoff between resolution and holding torque.

A 5mm pitch will get you .0001 inch steps if you microstep it 10x.  But you are losing some holding torque by chopping the steps that much.

When I sent mine up in Linux CNC there's a testing menu where you can run it at whatever speed you want then you can monitor for missed steps

Link to comment
Share on other sites

So I found this:

Inch PV Value Calculator | Nook Industries

And this:

Lead Screw Torque and Force Calculator (daycounter.com)

Working backwards, I know my stepper is rated for 2Nm holding torque and it is geared down 1:2. Assuming the nut is brass and CoF is 1.2, that means I can deliver 1200lbs before stalling the motor.

So the next question is, how much force can the M10x1.0 brass nut absorb?

  • Like 1
Link to comment
Share on other sites
  • 1 month later...

Back on topic:

I've got an XCarve job coming up (cutting the switch and gauge holes in a piece of aluminum plate that will be the faceplate for my mill control panel) so I will be doing the machine definition for the XCarve and the postprocessor for GRBL over the XMas break. Yay!

  • Like 2
Link to comment
Share on other sites
  • 4 weeks later...

OK, I have successfully run some XCarve operations and have an idea now what GRBL doesn't like.

Here is a quick extract of a simple spot drill op:

%
O0000(MILL CONTROL PANEL OP 1 V2 - SPOT DRILL)
(DATE=DD-MM-YY - 31-12-21 TIME=HH:MM - 13:51)
(MCAM FILE - M:\DOCUMENTS\DENNIS\SOLIDWORKS PROJECTS\MILL CONTROL PANEL\MILL CONTROL PANEL.SLDPRT)
(NC FILE - D:\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM FOR SOLIDWORKS\MILL\NC\MILL CONTROL PANEL OP 1 V2 - SPOT DRILL.nc)
(MATERIAL - ALUMINUM MM - 2024)
( T2 | 1/4 SPOTDRILL | H2 )
G20
G0 G17 G40 G49 G80 G90
T2 M6
G0 G90 G54 X1.3118 Y1.9291 A0. S27153 M3
G43 H2 Z.5
G1 Z-.075 F27.17
G0 Z.5
X2.6118
G1 Z-.075 F27.17
G0 Z.5
M5
G91 G28 Z0.
G28 X0. Y0. A0.
M30
%

 

Now here's a list of things GRBL did not like:

1. O0000 on first line

2. G0 G17 G40 G49 G80 G90 - Didn't like G0 with no following, axis, doesn't understand G80

3. Doesn't support tool changes, so need to eliminate T2 M6 (could be an optional stop with an optional move to a manual tool change position)

4. G0 G90 G54 X1.3118 Y1.9291 A0. S27153 M3 - spurious G90 and G54. Spurious A0. S and M3 should be on separate line

5. G43 H2 Z.5 - Doesn't support G43

6. G91 G28 Z0. - I think this works (I deleted it for test run) should fully retract spindle

7. G28 X0. Y0. A0. - Spurious A0. Not entirely sure if this is the right place to end. Need to know where in post this is controlled

Should look like:

%
(MILL CONTROL PANEL OP 1 V2 - SPOT DRILL)
(DATE=DD-MM-YY - 31-12-21 TIME=HH:MM - 13:51)
(MCAM FILE - M:\DOCUMENTS\DENNIS\SOLIDWORKS PROJECTS\MILL CONTROL PANEL\MILL CONTROL PANEL.SLDPRT)
(NC FILE - D:\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM FOR SOLIDWORKS\MILL\NC\MILL CONTROL PANEL OP 1 V2 - SPOT DRILL.nc)
(MATERIAL - ALUMINUM MM - 2024)
( T2 | 1/4 SPOTDRILL | H2 )
G20
G17 G40 G49 G90 G54
S27153 M3
G0 X1.3118 Y1.9291 
Z.5
G1 Z-.075 F27.17
G0 Z.5
X2.6118
G1 Z-.075 F27.17
G0 Z.5
M5
G91 G28 Z0.
G28 X0. Y0.
M30
%

I'll dive into the post later and see what I can figure out, but I'd be happy to accept pointers if anyone was so inclined.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...