What's new
What's new

Solidworks CAM - Double Toolpaths

Joined
Jun 13, 2024
Location
Raleigh, NC
Hello machining community,

I'm looking for help with what ought to be a straightforward fix, but I am at a loss google-searching without results.

I am creating a part with a boss feature (this will eventually run through a chamfer bit and become a die cutting blade) out of aluminum.

1718281562792.png
After machining the initial setup, I realized I wanted the boss to be a bit thinner because the blade was too thick. Instead of redrawing the boss, I thought I could just offset the toolpath by -1mm (see setting below) to make it thinner.

1718281791939.png

This does partially produce the desired result, however it also maintains the original toolpath location. Now my toolpath takes twice as long!

Is there any way to get rid of the original toolpath when a side allowance is specified?


1718281817554.png

Thanks in advance!
 
sorry dont use SWCAM, I use HSMWorks in SW, so I cannot solve this for you.
But the power of CAM in SW is that with a quick change of dimentions of the part will update the toolpath with a regen. This is what I do or I set wear and then use the offset on the CNC control to adjust on the fly.
 
It’s not the “original tool path” that you’re seeing but it thinks that there is more material to remove and it’s taking two cuts. To control this click the settings box below the allowance box. In there you can specify the amount of stock to remove and step over. This will allow you to have just one cut or whatever you want.
 
It's more than likely your settings in Rough Passes, Cut Amount and Previous Allowance. Your -1mm exceeds your Cut Amount % so it's giving it a Rough Pass.

I typically set my Prev Allowance to .01" but try an change it to 0
 

Attachments

  • UntitledA.jpg
    UntitledA.jpg
    157 KB · Views: 9
That was very helpful 🙄
But he did say: "After machining the initial setup, I realized I wanted the boss to be a bit thinner because the blade was too thick. Instead of redrawing the boss, I thought I could just offset the toolpath by -1mm (see setting below) to make it thinner."

Isn't that why we use CAM inside of SW?
Don't you want the part correct size if you have to come back later down the road and machine another?
Hence my second line, figured others would chime in on how to use SWCAM\CAMWorks.
 
But he did say: "After machining the initial setup, I realized I wanted the boss to be a bit thinner because the blade was too thick. Instead of redrawing the boss, I thought I could just offset the toolpath by -1mm (see setting below) to make it thinner."

Isn't that why we use CAM inside of SW?
Don't you want the part correct size if you have to come back later down the road and machine another?
Hence my second line, figured others would chime in on how to use SWCAM\CAMWorks.
I honesty misread your first comment. I read it as "sorry DONT use SWCAM" - My apologizes.

But yes, that would be one way to do it, adjust the model in SW, unless its a non SW native file.

I actually don't ever adjust models, I make all my comp adjustments to the toolpath itself. I also don't make my own products, but I could see if this was something of your own and you were testing and adjusting, it would make sense to adjust the model accordingly.
 
Using negative allowances is going to cause you hardship in the future. Trust me on this one. Redraw the boss. Once you get handy with Solidworks CAM, you can leave the little bullshit hacks alone.
 
I honesty misread your first comment. I read it as "sorry DONT use SWCAM" - My apologizes.

But yes, that would be one way to do it, adjust the model in SW, unless its a non SW native file.

I actually don't ever adjust models, I make all my comp adjustments to the toolpath itself. I also don't make my own products, but I could see if this was something of your own and you were testing and adjusting, it would make sense to adjust the model accordingly.
Yes I should have put "I" before don't :o

like not putting comma in the correct place in a sentence, read totally wrong.....
 
Using negative allowances is going to cause you hardship in the future. Trust me on this one. Redraw the boss. Once you get handy with Solidworks CAM, you can leave the little bullshit hacks alone.
I agree that the best thing here is to fix the part but not with a blanket statement of never using a negative allowance. I often use an edge as a tool path for finishing a narrow top edge and use a negative allowance so the cutter hangs over some. It has its place.
 
Using negative allowances is going to cause you hardship in the future. Trust me on this one. Redraw the boss. Once you get handy with Solidworks CAM, you can leave the little bullshit hacks alone.
I use it a lot on unilateral tolerances depending on how the model is designed. It has its place.

I use the Move Face tool alot for dumb solids for things like this works great!
The issue I have had in the past with modifying a SLDPRT file is, when a feature is dimensioned off a feature you are adjusting, everything moves.
 
I use it a lot on unilateral tolerances depending on how the model is designed. It has its place.


The issue I have had in the past with modifying a SLDPRT file is, when a feature is dimensioned off a feature you are adjusting, everything moves.

Yep, Design Intent plays a big roll in how dimension changes effect how a model updates. I try to instill that to the students, sometimes to def ears, then they get it when the model blows up.
 
It’s not the “original tool path” that you’re seeing but it thinks that there is more material to remove and it’s taking two cuts. To control this click the settings box below the allowance box. In there you can specify the amount of stock to remove and step over. This will allow you to have just one cut or whatever you want.
It seems like this is an unavoidable safety feature of SolidWorks CAM. Using a negative side allowance is useful, as some have stated, if you are in a rapid prototyping scenario and just want to "try" different size cuts without making a permanent modification to the part geometry. SolidWorks appears to correctly assume that it needs to then take multiple passes around the perimeter to prevent tool breakage with a negative side allowance specified.

Thanks to all who contributed. This was a niche question and more of a curiosity than a need
 
It seems like this is an unavoidable safety feature of SolidWorks CAM. Using a negative side allowance is useful, as some have stated, if you are in a rapid prototyping scenario and just want to "try" different size cuts without making a permanent modification to the part geometry. SolidWorks appears to correctly assume that it needs to then take multiple passes around the perimeter to prevent tool breakage with a negative side allowance specified.

Thanks to all who contributed. This was a niche question and more of a curiosity than a need
This is where configurations soars! in an assembly you can drop as many as you need and then cut each config.. I do this all the time works great.
You could also just make a sketch and at the size you want the offset to be and use that to cut, do that alot too.

All I do is make prototypes on off's and have to tweek things from the students models and some of them are pretty bad, they weren't taught how to model very well in the SW class that they took their sophomore year in college and then they need to use SW their senior year after not using it for 2 years, But hey we getter done. I always go back to the way we did it in other CAM and try to mimic it inside of SW and whatever CAM inside, tricks tricks and more tricks.

the more you try other things the bigger your toolbox gets to finish the parts on the machine. it pays to be abused by the older softwares we cut our teeth on.
 
This is where configurations soars! in an assembly you can drop as many as you need and then cut each config.. I do this all the time works great.
You could also just make a sketch and at the size you want the offset to be and use that to cut, do that alot too.

All I do is make prototypes on off's and have to tweek things from the students models and some of them are pretty bad, they weren't taught how to model very well in the SW class that they took their sophomore year in college and then they need to use SW their senior year after not using it for 2 years, But hey we getter done. I always go back to the way we did it in other CAM and try to mimic it inside of SW and whatever CAM inside, tricks tricks and more tricks.

the more you try other things the bigger your toolbox gets to finish the parts on the machine. it pays to be abused by the older softwares we cut our teeth on.
Agree, configurations work great! I resort to sketches, more than anything, occasionally surfaces. I find it nice to create the sketch, name it and be able to easily reference it and know what the toolpath "modification" is.
 
It seems like this is an unavoidable safety feature of SolidWorks CAM. Using a negative side allowance is useful, as some have stated, if you are in a rapid prototyping scenario and just want to "try" different size cuts without making a permanent modification to the part geometry. SolidWorks appears to correctly assume that it needs to then take multiple passes around the perimeter to prevent tool breakage with a negative side allowance specified.

Thanks to all who contributed. This was a niche question and more of a curiosity than a need
I hate software that "assumes" things or has "unavoidable safety features". An offer to help is sometimes nice, a notification that the tool is gouging the part is great, but when the software starts forcefully inserting things I don't want or need, that's when I start shopping for other software.
 
I hate software that "assumes" things or has "unavoidable safety features". An offer to help is sometimes nice, a notification that the tool is gouging the part is great, but when the software starts forcefully inserting things I don't want or need, that's when I start shopping for other software.
This is not an assumed setting by CAMWorks/SWCAM, nor is it a forced parameter that is inserted for any sort of safety feature.

By default I believe the Cut Amount is set to 40% of tool diameter, so when you put a negative offset value in greater than 40% of the tool diameter it creates an additional step over, based on the default setting. Which can easily be changed or adjusted.
 








 
Back
Top