Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Chamfer Help

20 REPLIES 20
Reply
Message 1 of 21
fiona6S9UQ
653 Views, 20 Replies

Chamfer Help

I am having problems sending programs out to chamfer.

On the machines we use a radius offset of 1.5mm on the machines as a standard.

The shop floor wants the code to post in comp which ive found in control sends the code out properly with the compensation but for some reason, no matter what i try the chamfering doesnt work. It either machines nothing or to much and im not sure exactly how to go about it.

 

I am using a 2D contour with in control as compensation type. I select the boundary to follow (Bottom of chamfer) and set the Z top and bottom to the top surface of the chamfer. 

 

I add an offset to the bottom height to create the depth i require. For example for a 0.25mm chamfer i put 1.25mm bottom depth.

 

The code looks correct when posting it but its not working out on the shop floor.

Is there anything i need to keep an eye on and make sure is checked to properly chamfer?

20 REPLIES 20
Message 2 of 21
seth.madore
in reply to: fiona6S9UQ

Would you be able to share your Fusion file here?
File > Export > Save to local folder, return to thread and attach the .f3d/.f3z file in your reply.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 21
fiona6S9UQ
in reply to: fiona6S9UQ

Here is the file attached. I am not sure if i am using the right post processor but even looking at the posted code it all looks correct.
The machines use Heidenhain 540 control so not sure if the post processor could be it, as i am not sure which is the correct one to use.

 

Ive been using the normal Heidenhain post processor but i see there is a ISO post processor.

Message 4 of 21
seth.madore
in reply to: fiona6S9UQ

Hmm, I'm not sure on which post processor. Looking at Heidenhain's website, I'm not seeing documentation for the 540 control, but do for the 640 🤔


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 21
fiona6S9UQ
in reply to: fiona6S9UQ

It looks like the Heidenhain.cps post processor may be the correct one as in the post description it says "longDescription = "Generic post for Heidenhain controls like iTNC 530, TNC 620, and TNC 640.";"

 

I am hoping to get onto a machine in the next week to mess around with the chamfer. The previous programmer used in computer and gave no ability to the machinists on the floor to adjust the chamfer. Trying to find a way round it but not being able to run my own programs it makes it difficult to impossible to see what changes affect what.

Message 6 of 21
seth.madore
in reply to: fiona6S9UQ

Ahh, so I'm looking at your file now. You've got some things set wrong...

Selection: When working with modeled chamfers, we want to be selecting the top edge (which you did). That said, both 2D Contour (with chamfer) and the Chamfer toolpath are much easier to use when the chamfers are not modeled. Just a tip 😉

Heights: Bottom Height should be set to "Selected Contour"

Passes: Turn on "Chamfer", set Chamfer size to zero and the Bottom Height Offset to whatever you would like the tool to drop down by.

 

Now, the in-canvas display of the toolpath is going to look a bit "off", as it's inset into the part:

2024-03-15_04h33_52.png

When we hop into Simulation, we see the corrected result:

2024-03-15_04h34_29.png

 (this is one of the many reasons I'm not a fan of In-Control, but I respect that others feel differently)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 21
seth.madore
in reply to: fiona6S9UQ

Clarification on the contour selection and Chamfer tip offset:

1) Your selections were on the bottom edge, we want the top edge

2) Your Chamfer tip offset needs to be at least your chamfer size plus whatever offset you desire. So, if it's a 1mm chamfer and you want the tip to go below the edge by another 1mm, you need to have a Chamfer Tip Offset of 2mm.

These are not reflected in the file I shared back to you in my prior post!


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 8 of 21

If you are trying to machine using the 'In Control' option and using G41/G42 you need to make sure the physical tool you are using matches the tool defined on your machine in the offsets page The radius and the orientation of the tool, if incorrect will have an impact on chamfers and diameters. That's what I would check first anyway if my code looks correct.

Christopher Cooper
Technical Consultant
Message 9 of 21
Tomas_V_cz
in reply to: fiona6S9UQ

if possible, don't use chamfer tool correction. Use compensation type: in computer and simulation and real will be 1:1. what radius do you enter in the tool table on the CNC machine? Large diameter of the tool /2 , small diameter /2 (which is 0) , diameter at the point of contact /2 ?

Save yourself the worry if possible. In case you use the compensation type: in the computer, it will not affect what data you enter in the table as the radius and the path will always be good

Message 10 of 21

We program as In Computer. If user needs to adjust (they dont with proper programming! Our chamfer mills have a .005 tip dia) you just use a Z length offset to make it bigger if required. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 11 of 21


@programming2C78B wrote:

...you just use a Z length offset to make it bigger if required. 


Agreed, but sometimes that's not always an option, especially when running close to a bottom edge/face


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 12 of 21
fiona6S9UQ
in reply to: seth.madore

I have applied the changes you suggested to the model. Its done as you mentioned that on screen it looks wrong but running it through simulation it looks fine.

The problem comes that when i post the code its wrong. 

It should comp into X-71.475 and go round but the code is coming out comping into X-63.85 which is what the tool path before simulation looks like. 

Unless there is something additional i am doing wrong.

Message 13 of 21

The previous programmer done all the chamfers in computer but out on the shop floor we weren't able to adjust the chamfers to how we wanted. Which is why management is requesting that its posted in control.

 

To mention ive only used Fusion a few times and been tasked with getting it to work for our company so is stressful.

Message 14 of 21
Tomas_V_cz
in reply to: fiona6S9UQ

if you have a tool in Fusion that is the same as a real machining tool, there is no reason for the tool not to machine the edge as needed. Examine the tool geometry and discover why the path differs from the simulation. The CNC operator will still be able to make a small adjustment to the chamfer. They will only adjust the length of the tool.

Convince the shop management (if possible) that it is better to use the type of compensation: in the computer for the chamfering operation.

Message 15 of 21
seth.madore
in reply to: fiona6S9UQ


@fiona6S9UQ wrote:

I have applied the changes you suggested to the model. Its done as you mentioned that on screen it looks wrong but running it through simulation it looks fine.

The problem comes that when i post the code its wrong. 

It should comp into X-71.475 and go round but the code is coming out comping into X-63.85 which is what the tool path before simulation looks like. 

Unless there is something additional i am doing wrong.


And what radius/diameter value are you putting in the control for this tool?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 16 of 21
fiona6S9UQ
in reply to: seth.madore

1.5 Radius in the tool table which is why for a 0.5mm chamfer i go Z-1.5.
Interestingly i am chamfering some bores.

Putting the compensation type makes the graphics look good but not the adjustability we need for the workshop.

Putting the compensation into control the graphics show a straight line but the code is coming out correct.

Message 17 of 21
seth.madore
in reply to: fiona6S9UQ

Your chamfer tool measures 16mm in diameter, you should be putting in a value of 8mm into your control as a starting number. From your numbers above, there's a 7.625mm difference between your code and what you expect to see at the machine.

The 8mm value does not take into account the .75mm flat on the end of the tool, so you'll likely need to reduce the offset amount to account for that size difference


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 18 of 21

is there a reason you cant just model the tool as 16mm with the .75mm flat, and use Wear comp on the machine? 

Please click "Accept Solution" if what I wrote solved your issue!
Message 19 of 21
RickDuckworth
in reply to: seth.madore

@seth.madore, you say to always select the top edge of the chamfer when it is modeled. Can you explain why the top edge is better?

I always select the bottom edge of the chamfer when it is modeled because that's the way I was taught. I have never had an issue doing it this way. I agree it is much easier when the chamfer isn't modeled. 

Message 20 of 21
seth.madore
in reply to: RickDuckworth


@RickDuckworth wrote:

@seth.madore, you say to always select the top edge of the chamfer when it is modeled. Can you explain why the top edge is better?

I always select the bottom edge of the chamfer when it is modeled because that's the way I was taught. I have never had an issue doing it this way. I agree it is much easier when the chamfer isn't modeled. 


There have been errors (historically) of selecting the bottom edge and getting a less than adequate result. It's possible those issues have been solved, I just tend to go with what I know will work. If bottom edge works in all cases, than by all means, go with that.


Seth Madore
Customer Advocacy Manager - Manufacturing

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report